[OpenFOAM] ./Allrun: 24: ./Allrun: cannot create /opt/openfoam220/etc/controlDict:

Mirage12 · May 22, 2013, 02:42

Hello everyone

I am a new OpenFoam user and try to understand the tutorial cylinder :

Code:

/tutorials/basic/potentialFoam/cylinder

, but I have same problems to run it.

I cannot create the regular file `/opt/openfoam220/etc/controlDict.3364'

After typing the command

Code:

./Allrun

in the terminal, i got this Error :

Code:

Modifying /opt/openfoam220/etc/controlDict to enable allowSystemOperations
cp: cannot create regular file `/opt/openfoam220/etc/controlDict.3364': Permission denied
Enabling allowSystemOperations in /opt/openfoam220/etc/controlDict.  
./Allrun: 24: ./Allrun: cannot create /opt/openfoam220/etc/controlDict: Permission denied
Running blockMesh on /home/abm5kor/cylinder
Running potentialFoam on /home/abm5kor/cylinder
Running streamFunction on /home/abm5kor/cylinder

And after typing the command paraFoam, i got this error :

Code:

ERROR: In /home/kitware/Dashboards/MyTests/ParaView-master/VTK/IO/vtkOpenFOAMReader.cxx, line 4639
vtkOpenFOAMReaderPrivate (0x201a8f0): Error opening /home/abm5kor/cylinder/constant/polyMesh/faces.gz: Can't open. If you are trying to read a parallel decomposed case, set Case Type to Decomposed Case.


ERROR: In /home/kitware/Dashboards/MyTests/ParaView-master/VTK/Filtering/vtkExecutive.cxx, line 756
vtkPVCompositeDataPipeline (0x20022e0): Algorithm vtkPOpenFOAMReader(0x20101e0) returned failure for request: vtkInformation (0x21ea340)
  Debug: Off
  Modified Time: 96685
  Reference Count: 1
  Registered Events: (none)
  Request: REQUEST_DATA
  FORWARD_DIRECTION: 0
  ALGORITHM_AFTER_FORWARD: 1
  FROM_OUTPUT_PORT: 0

I can Apply the file but i cannot see anything "the cylinder".

How can i solve this problem ?

Thank you so much!!!!!!!!!!!!!!!!!

Mirage12 · May 23, 2013, 01:10

Quote:

Originally Posted by Mirage12

Hello everyone

I am a new OpenFoam user and try to understand the tutorial cylinder :

Code:

/tutorials/basic/potentialFoam/cylinder

, but I have same problems to run it.

I cannot create the regular file `/opt/openfoam220/etc/controlDict.3364'

After typing the command

Code:

./Allrun

in the terminal, i got this Error :

Code:

Modifying /opt/openfoam220/etc/controlDict to enable allowSystemOperations
cp: cannot create regular file `/opt/openfoam220/etc/controlDict.3364': Permission denied
Enabling allowSystemOperations in /opt/openfoam220/etc/controlDict.  
./Allrun: 24: ./Allrun: cannot create /opt/openfoam220/etc/controlDict: Permission denied
Running blockMesh on /home/abm5kor/cylinder
Running potentialFoam on /home/abm5kor/cylinder
Running streamFunction on /home/abm5kor/cylinder

And after typing the command paraFoam, i got this error :

Code:

ERROR: In /home/kitware/Dashboards/MyTests/ParaView-master/VTK/IO/vtkOpenFOAMReader.cxx, line 4639
vtkOpenFOAMReaderPrivate (0x201a8f0): Error opening /home/abm5kor/cylinder/constant/polyMesh/faces.gz: Can't open. If you are trying to read a parallel decomposed case, set Case Type to Decomposed Case.


ERROR: In /home/kitware/Dashboards/MyTests/ParaView-master/VTK/Filtering/vtkExecutive.cxx, line 756
vtkPVCompositeDataPipeline (0x20022e0): Algorithm vtkPOpenFOAMReader(0x20101e0) returned failure for request: vtkInformation (0x21ea340)
  Debug: Off
  Modified Time: 96685
  Reference Count: 1
  Registered Events: (none)
  Request: REQUEST_DATA
  FORWARD_DIRECTION: 0
  ALGORITHM_AFTER_FORWARD: 1
  FROM_OUTPUT_PORT: 0

I can Apply the file but i cannot see anything "the cylinder".

How can i solve this problem ?

Thank you so much!!!!!!!!!!!!!!!!!

Any idea how to solve my problem ?

I use Linux 12.04 and OpenFOAM 2.20

I need your help.

Thanks in advance,

ngj · May 23, 2013, 04:22

Hi Amin,

You are executing the tutorial in the root of the operating system, where you do not have permission to alter or add new files. Copy the entire tutorial folder to a location in your home directory, and you should be allowed to run the tutorials.

Kind regards

Niels

Mirage12 · May 23, 2013, 05:33

Quote:

Originally Posted by ngj

Hi Amin,

You are executing the tutorial in the root of the operating system, where you do not have permission to alter or add new files. Copy the entire tutorial folder to a location in your home directory, and you should be allowed to run the tutorials.

Kind regards

Niels

Thank you so munch for your answer.

I copied the tutorial to location in my home directory, but i still have the same error.
i did already the tutorial airfoil2d and cavity without any problems and i didn't receive this error....

ngj · May 23, 2013, 06:40

Hi,

Sorry, I was a bit quick in my answer, since I mostly focused on the "permission denied" part of the error.

The tutorial changes some options in the file

Code:

/opt/openfoam220/etc/controlDict

but since changes to this file are not permitted in the root directory, then you cannot execute the tutorial. I am not using 2.2.0 myself, so I do not know, what "codeStream" mentioned in the Allrun script does.

One option is to (i) manually change the file /opt/openfoam220/etc/controlDict and then (ii) remove the relevant parts from the Allrun. Another option is to understand what codeStream does and remove it from the simulation.

A third option is to enforce changes by the script by executing

Code:

sudo ./Allrun

which will ask for your password and then you can potentially change everything in the root file system. If you are not familiar with the sudo command, please do read a bit about it, before you start using it.

Kind regards

Niels

haakon · May 23, 2013, 07:46

I Think the answer lies in the allowSystemOperations switch in the etc/controlDict. This must be set to "1" for the cylinder tutorial to work, as it uses run-time compiled C++ objects.

So, as root, change the allow SystemOperations value in etc/controlDict form 0 to 1, and you are good to go.

For reference, this is how it should look like:

Code:

InfoSwitches
{
    writePrecision  6;
    writeJobInfo    0;
    writeDictionaries 0;

    // Allow case-supplied C++ code (#codeStream, codedFixedValue)
    allowSystemOperations   1;
}

Mirage12 · May 23, 2013, 08:47

Thanks for your answer !

I tried to bluid the with blockMesh... but i received an Error.

Code:

--> FOAM FATAL IO ERROR:
ill defined primitiveEntry starting at keyword '|' on line 1 and ending at line 1028
file: /opt/openfoam220/etc/controlDict at line 1028.

    From function primitiveEntry::readEntry(const dictionary&, Istream&)
    in file db/dictionary/primitiveEntry/primitiveEntryIO.C at line 190

.

I think haakon is right

but i couldn't save the modification...because controlDict is in the file system..so how can save the change ?

can you please explain why should i change the 0 to 1 ?

Thanks a lot

haakon · May 23, 2013, 09:06

First; you need to do the change as root. If you do not have that access, ask your system administrator to do the change for you (they are usually really nice and helpful).

Second; you should change from 0 to 1 to allow OpenFOAM to build C++ code attached in the input files. See for example the code in tutorials/basic/potentialFoam/cylinder/system/controlDict as an example. It contain source code that needs to be compiled in order to work. The allowSystemOperations switch control this, if it 0 you are not allowed to build and execute source code from within the OpenFOAM input files.

Mirage12 · May 23, 2013, 09:23

I changed the file and i can build the mesh using the command blockMesh, without any problems

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0-b363e8d14789
Exec   : blockMesh
Date   : May 23 2013
Time   : 17:49:11
Host   : "BMH301562"
PID    : 10470
Case   : /home/abm5kor/cylinder
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

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

Creating block mesh from
    "/home/abm5kor/cylinder/constant/polyMesh/blockMeshDict"
Using #codeStream at line 19 in file "/home/abm5kor/cylinder/constant/polyMesh/blockMeshDict"
Using #codeStream with "/home/abm5kor/cylinder/dynamicCode/platforms/linux64GccDPOpt/lib/libcodeStream_1c19e29ae18c779aa836a14631d6419f303e3d9d.so"
Creating new library in "dynamicCode/_1c19e29ae18c779aa836a14631d6419f303e3d9d/platforms/linux64GccDPOpt/lib/libcodeStream_1c19e29ae18c779aa836a14631d6419f303e3d9d.so"
Invoking "wmake -s libso /home/abm5kor/cylinder/dynamicCode/_1c19e29ae18c779aa836a14631d6419f303e3d9d"
wmakeLnInclude: linking include files to ./lnInclude
Making dependency list for source file codeStreamTemplate.C
'/home/abm5kor/cylinder/dynamicCode/_1c19e29ae18c779aa836a14631d6419f303e3d9d/../platforms/linux64GccDPOpt/lib/libcodeStream_1c19e29ae18c779aa836a14631d6419f303e3d9d.so' is up to date.
Creating curved edges
Creating topology blocks
Creating topology patches

Creating block mesh topology
--> FOAM Warning : 
    From function polyMesh::polyMesh(... construct from shapes...)
    in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 901
    Found 20 undefined faces in mesh; adding to default patch.

Check topology

    Basic statistics
        Number of internal faces : 12
        Number of boundary faces : 36
        Number of defined boundary faces : 36
        Number of undefined boundary faces : 0
    Checking patch -> block consistency

Creating block offsets
Creating merge list .

Creating polyMesh from blockMesh
Creating patches
Creating cells
Creating points with scale 1

Writing polyMesh
----------------
Mesh Information
----------------
  boundingBox: (-2 0 -0.5) (2 2 0.5)
  nPoints: 4222
  nCells: 2000
  nFaces: 8110
  nInternalFaces: 3890
----------------
Patches
----------------
  patch 0 (start: 3890 size: 60) name: down
  patch 1 (start: 3950 size: 30) name: right
  patch 2 (start: 3980 size: 60) name: up
  patch 3 (start: 4040 size: 30) name: left
  patch 4 (start: 4070 size: 40) name: cylinder
  patch 5 (start: 4110 size: 4000) name: defaultFaces

End

but when i type the command

Code:

./Allrun

i receive this error :

Code:

Modifying /opt/openfoam220/etc/controlDict to enable allowSystemOperations
cp: cannot create regular file `/opt/openfoam220/etc/controlDict.10578': Permission denied
Enabling allowSystemOperations in /opt/openfoam220/etc/controlDict.
./Allrun: 24: ./Allrun: cannot create /opt/openfoam220/etc/controlDict: Permission denied
Running blockMesh on /home/abm5kor/cylinder
Running potentialFoam on /home/abm5kor/cylinder
Running streamFunction on /home/abm5kor/cylinder

thank you for your support

haakon · May 23, 2013, 09:35

After having looked on the Allrun script myself, I don't think you should worry. The only thing it that part does is to change the allowSystemOperations from 0 to 1... Since you have already done that part, everything is hopefully fine. Are the results reasonable?

Mirage12 · May 23, 2013, 10:26

Quote:

Originally Posted by haakon

After having looked on the Allrun script myself, I don't think you should worry. The only thing it that part does is to change the allowSystemOperations from 0 to 1... Since you have already done that part, everything is hopefully fine. Are the results reasonable?

Not Really.....

when i write the commd

Code:

potentialFoam

I receive this Error :

Code:

Create time

Create mesh for time = 0

Reading field p



--> FOAM FATAL IO ERROR: 
cannot find file

file: /home/abm5kor/cylinder/0/p at line 0.

    From function regIOobject::readStream()
    in file db/regIOobject/regIOobjectRead.C at line 73.

FOAM exiting

and when i write the command

Code:

streamFunction

I receive this Error :

Code:

Create time



--> FOAM FATAL ERROR: 
No times selected

    From function streamFunction
    in file db/Time/timeSelector.C at line 263.

FOAM exiting

wyldckat · May 25, 2013, 15:12

Greetings to all!

@Amin: If you look into the script file "Allrun", you'll see the instructions that should be used for running this example case. You can also seem it online here: https://github.com/OpenFOAM/OpenFOAM...ylinder/Allrun

Since you now have the "allowSystemOperations" configured, then all that's left is to do the following commands:

Code:

cp -r 0.org 0
blockMesh
potentialFoam
streamFunction

It's the first command that you are missing, which copies the "0.org" folder to "0".

Best regards,
Bruno

Mirage12 · May 27, 2013, 05:35

Hello Bruno

Thanks for your help.

I can build the Mesh !!!

But

i still have a problem with this 2 commands
potentialFoam streamFunction
After typing the 2 commands, i did not get any errors....but after opening Paraview and applying the file, i got this Error :

Code:

ERROR: In /home/kitware/Dashboards/MyTests/ParaView-master/VTK/IO/vtkOpenFOAMReader.cxx, line 6538
vtkOpenFOAMReaderPrivate (0x2a2e290): Wrong list type for uniform field


ERROR: In /home/kitware/Dashboards/MyTests/ParaView-master/VTK/IO/vtkOpenFOAMReader.cxx, line 4471
vtkOpenFOAMReaderPrivate (0x31a3560): Error reading line 58 of /home/abm5kor/potentialFoam/cylinder/system/controlDict: Unsupported directive {


ERROR: In /home/kitware/Dashboards/MyTests/ParaView-master/VTK/Filtering/vtkExecutive.cxx, line 756
vtkPVCompositeDataPipeline (0x2a16710): Algorithm vtkPOpenFOAMReader(0x2a16b90) returned failure for request: vtkInformation (0x2a2e930)
  Debug: Off
  Modified Time: 92279
  Reference Count: 1
  Registered Events: (none)
  Request: REQUEST_INFORMATION
  FORWARD_DIRECTION: 0
  ALGORITHM_AFTER_FORWARD: 1

Here ist the ouptput of

Code:

potentialFoam

:

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0-b363e8d14789
Exec   : potentialFoam
Date   : May 27 2013
Time   : 13:43:50
Host   : "BMH301562"
PID    : 8259
Case   : /home/abm5kor/potentialFoam/cylinder
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

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

Create mesh for time = 0

Reading field p

Reading field U


Calculating potential flow
Using dynamicCode for functionObject difference at line 53 in "/home/abm5kor/potentialFoam/cylinder/system/controlDict.functions.difference"
Creating new library in "dynamicCode/error/platforms/linux64GccDPOpt/lib/liberror_e92448da6ae10bc777e0869670f72a48fd0673f1.so"
Invoking "wmake -s libso /home/abm5kor/potentialFoam/cylinder/dynamicCode/error"
wmakeLnInclude: linking include files to ./lnInclude
Making dependency list for source file functionObjectTemplate.C
Making dependency list for source file FilterFunctionObjectTemplate.C
'/home/abm5kor/potentialFoam/cylinder/dynamicCode/error/../platforms/linux64GccDPOpt/lib/liberror_e92448da6ae10bc777e0869670f72a48fd0673f1.so' is up to date.
DICPCG:  Solving for p, Initial residual = 1, Final residual = 7.87069e-07, No Iterations 76
DICPCG:  Solving for p, Initial residual = 0.0126096, Final residual = 7.71198e-07, No Iterations 64
DICPCG:  Solving for p, Initial residual = 0.0025829, Final residual = 9.49278e-07, No Iterations 59
DICPCG:  Solving for p, Initial residual = 0.000902306, Final residual = 8.48077e-07, No Iterations 57
continuity error = 3.37204e-05
Interpolated U error = 1.20218e-05
Looking up field U

Reading inlet velocity  uInfX

U at inlet = 1 m/s
Cylinder radius = 0.499614 m

Evaluating analytical solution
Writing relative error in U to "/home/abm5kor/potentialFoam/cylinder/0/error"
ExecutionTime = 0.13 s  ClockTime = 13 s

End

i did not find the file #kitware#

here is the controlDict-File

https://github.com/OpenFOAM/OpenFOAM...ontrolDict#L27

and here is the output of

Code:

 streamFunction

:

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0-b363e8d14789
Exec   : streamFunction
Date   : May 27 2013
Time   : 13:44:12
Host   : "BMH301562"
PID    : 8339
Case   : /home/abm5kor/potentialFoam/cylinder
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

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

Create mesh for time = 0


Time: 0

Reading field phi
Zero face: patch: 0    face: 0
.......................................

End

I think, that

Code:

potentialFoam

calculated nothing...

any idea

Thanks

wyldckat · May 27, 2013, 18:08

Hi Amin,

It looks like it's only ParaView which is having a hard time understanding how to open the case.

Which exact version of ParaView are you using and how did you install it?

Best regards,
Bruno

Mirage12 · May 28, 2013, 03:38

i am using ParaView-3.12.0-Linux-x86_64 and Ubuntu 12.04 and downloaded it from the website of ParaView http://www.paraview.org/paraview/resources/software.php

Thanks for your support

wyldckat · May 28, 2013, 19:28

Hi Amin,

I was not able to reproduce the same error. So here are a few suggestions:

If you have not yet done the "cavity" tutorial from the User Guide, I suggest that you do it, to confirm if ParaView is working properly.
Copy the "system/controlDict" file to "system/controlDict.original". Then edit the file "system/controlDict" and remove everything below and including the line "functions". Save and close the file. Then run ParaView once again.

If either one of these suggestions still give you an error, then there is something else going on that is causing the problems.

Best regards,
Bruno

Mirage12 · May 29, 2013, 01:30

Hey Bruno

i did already the cavity and airfoil2d tutorial without any problems.

the input of my system/controlDict ist now:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     potentialFoam;

startFrom       startTime;

startTime       0;

stopAt          endTime;

endTime         1;

deltaT          1;

writeControl    timeStep;

writeInterval   1;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression off;

timeFormat      general;

timePrecision   6;

runTimeModifiable true;


// ************************************************************************* //

and i received the same error :

Code:

ERROR: In /home/kitware/Dashboards/MyTests/ParaView-master/VTK/IO/vtkOpenFOAMReader.cxx, line 6538
vtkOpenFOAMReaderPrivate (0x22d7900): Wrong list type for uniform field


ERROR: In /home/kitware/Dashboards/MyTests/ParaView-master/VTK/IO/vtkOpenFOAMReader.cxx, line 6538
vtkOpenFOAMReaderPrivate (0x22d7900): Wrong list type for uniform field

wyldckat · May 29, 2013, 19:00

Hi Amin,

OK, I finally managed to figure it out.
The problem is due to this in the "0/U" file:

Code:

    left
    {
        type            uniformFixedValue;
        uniformValue    constant (1 0 0);
    }

This is very different from what ParaView's internal ".foam" reader is expecting:

Code:

    left
    {
        type            uniformFixedValue;
        uniformValue    uniform (1 0 0);
    }

Problem is that this second form will not work with OpenFOAM.

But the following should work for both OpenFOAM and ParaView:

Code:

    left
    {
        type            uniformFixedValue;
        uniformValue    (1 0 0);
    }

Keep in mind to edit the file "0.org/U" and perform all of the steps for executing once again!

Best regards,
Bruno

Mirage12 · May 30, 2013, 11:09

Hello Bruno

The Error is gone

but i think that potentialFoam is not working because the solver doesn’t calculate the velocity, pressure and the other variables for other delta T (Time)....

here ist output of potentialFoam:

Code:

Create time

Create mesh for time = 0

Reading field p

Reading field U


Calculating potential flow
Using dynamicCode for functionObject difference at line 53 in "/home/abm5kor/tutorials/basic/potentialFoam/cylinder/system/controlDict.functions.difference"
Creating new library in "dynamicCode/error/platforms/linux64GccDPOpt/lib/liberror_e92448da6ae10bc777e0869670f72a48fd0673f1.so"
Invoking "wmake -s libso /home/abm5kor/tutorials/basic/potentialFoam/cylinder/dynamicCode/error"
wmakeLnInclude: linking include files to ./lnInclude
Making dependency list for source file functionObjectTemplate.C
Making dependency list for source file FilterFunctionObjectTemplate.C
'/home/abm5kor/tutorials/basic/potentialFoam/cylinder/dynamicCode/error/../platforms/linux64GccDPOpt/lib/liberror_e92448da6ae10bc777e0869670f72a48fd0673f1.so' is up to date.
DICPCG:  Solving for p, Initial residual = 1, Final residual = 7.87069e-07, No Iterations 76
DICPCG:  Solving for p, Initial residual = 0.0126096, Final residual = 7.71198e-07, No Iterations 64
DICPCG:  Solving for p, Initial residual = 0.0025829, Final residual = 9.49278e-07, No Iterations 59
DICPCG:  Solving for p, Initial residual = 0.000902306, Final residual = 8.48077e-07, No Iterations 57
continuity error = 3.37204e-05
Interpolated U error = 1.20218e-05
Looking up field U

Reading inlet velocity  uInfX

U at inlet = 1 m/s
Cylinder radius = 0.499614 m

Evaluating analytical solution
Writing relative error in U to "/home/abm5kor/tutorials/basic/potentialFoam/cylinder/0/error"
ExecutionTime = 0.11 s  ClockTime = 13 s

End

OpenFoam did not generate other file's time...

why ?

Mirage12 · May 31, 2013, 07:34

Hey Bruno

i tried to run the Tutorial

Code:

heatTransfer/buoyantSimpleFoam/circuitBoardCooling

but i become the same error, when i start ParaView.

here is the message of the error :

Code:

ERROR: In /home/kitware/Dashboards/MyTests/ParaView-master/VTK/IO/vtkOpenFOAMReader.cxx, line 6882
vtkOpenFOAMReaderPrivate (0x3259da0): boundaryField region0_to_baffleRegion_baffleFaces2_top not found in object T at time = 0


ERROR: In /home/kitware/Dashboards/MyTests/ParaView-master/VTK/IO/vtkOpenFOAMReader.cxx, line 6882
vtkOpenFOAMReaderPrivate (0x3259da0): boundaryField region0_to_baffleRegion_baffleFaces2_top not found in object U at time = 0


ERROR: In /home/kitware/Dashboards/MyTests/ParaView-master/VTK/IO/vtkOpenFOAMReader.cxx, line 6882
vtkOpenFOAMReaderPrivate (0x3259da0): boundaryField region0_to_baffleRegion_baffleFaces2_top not found in object alphat at time = 0


ERROR: In /home/kitware/Dashboards/MyTests/ParaView-master/VTK/IO/vtkOpenFOAMReader.cxx, line 6882
vtkOpenFOAMReaderPrivate (0x3259da0): boundaryField region0_to_baffleRegion_baffleFaces2_top not found in object epsilon at time = 0


ERROR: In /home/kitware/Dashboards/MyTests/ParaView-master/VTK/IO/vtkOpenFOAMReader.cxx, line 6882
vtkOpenFOAMReaderPrivate (0x3259da0): boundaryField region0_to_baffleRegion_baffleFaces2_top not found in object k at time = 0


ERROR: In /home/kitware/Dashboards/MyTests/ParaView-master/VTK/IO/vtkOpenFOAMReader.cxx, line 6882
vtkOpenFOAMReaderPrivate (0x3259da0): boundaryField region0_to_baffleRegion_baffleFaces2_top not found in object mut at time = 0


ERROR: In /home/kitware/Dashboards/MyTests/ParaView-master/VTK/IO/vtkOpenFOAMReader.cxx, line 6882
vtkOpenFOAMReaderPrivate (0x3259da0): boundaryField region0_to_baffleRegion_baffleFaces2_top not found in object p at time = 0


ERROR: In /home/kitware/Dashboards/MyTests/ParaView-master/VTK/IO/vtkOpenFOAMReader.cxx, line 6882
vtkOpenFOAMReaderPrivate (0x3259da0): boundaryField region0_to_baffleRegion_baffleFaces2_top not found in object p_rgh at time = 0


ERROR: In /home/kitware/Dashboards/MyTests/ParaView-master/VTK/IO/vtkOpenFOAMReader.cxx, line 6882
vtkOpenFOAMReaderPrivate (0x32a16a0): boundaryField floor not found in object Q at time = 0


ERROR: In /home/kitware/Dashboards/MyTests/ParaView-master/VTK/IO/vtkOpenFOAMReader.cxx, line 6882
vtkOpenFOAMReaderPrivate (0x32a16a0): boundaryField region0_to_baffleRegion_baffleFaces2_top not found in object T at time = 0


ERROR: In /home/kitware/Dashboards/MyTests/ParaView-master/VTK/IO/vtkOpenFOAMReader.cxx, line 6882
vtkOpenFOAMReaderPrivate (0x32a16a0): boundaryField floor not found in object p at time = 0

i think, i should change this

Code:

left     
{        
 type            
uniformFixedValue;         uniformValue    constant (1 0 0);     
}

but also something else....... but i don’t know, really , what i should do !!

could you please help me ?

PS: i am using OpenFoam 2.2.0

May 23, 2013, 07:46		#6
haakon Senior Member Join Date: Dec 2011 Posts: 111 Rep Power: 20	I Think the answer lies in the allowSystemOperations switch in the etc/controlDict. This must be set to "1" for the cylinder tutorial to work, as it uses run-time compiled C++ objects. So, as root, change the allow SystemOperations value in etc/controlDict form 0 to 1, and you are good to go. For reference, this is how it should look like: Code: InfoSwitches { writePrecision 6; writeJobInfo 0; writeDictionaries 0; // Allow case-supplied C++ code (#codeStream, codedFixedValue) allowSystemOperations 1; } Mirage12 likes this.

May 23, 2013, 09:35		#10
haakon Senior Member Join Date: Dec 2011 Posts: 111 Rep Power: 20	After having looked on the Allrun script myself, I don't think you should worry. The only thing it that part does is to change the allowSystemOperations from 0 to 1... Since you have already done that part, everything is hopefully fine. Are the results reasonable? Mirage12 likes this.

May 25, 2013, 15:12		#12
wyldckat Retired Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,981 Blog Entries: 45 Rep Power: 128	Greetings to all! @Amin: If you look into the script file "Allrun", you'll see the instructions that should be used for running this example case. You can also seem it online here: https://github.com/OpenFOAM/OpenFOAM...ylinder/Allrun Since you now have the "allowSystemOperations" configured, then all that's left is to do the following commands: Code: cp -r 0.org 0 blockMesh potentialFoam streamFunction It's the first command that you are missing, which copies the "0.org" folder to "0". Best regards, Bruno __________________ OpenFOAM: FAQ \| Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM

May 27, 2013, 18:08		#14
wyldckat Retired Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,981 Blog Entries: 45 Rep Power: 128	Hi Amin, It looks like it's only ParaView which is having a hard time understanding how to open the case. Which exact version of ParaView are you using and how did you install it? Best regards, Bruno __________________ OpenFOAM: FAQ \| Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM

May 28, 2013, 19:28		#16
wyldckat Retired Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,981 Blog Entries: 45 Rep Power: 128	Hi Amin, I was not able to reproduce the same error. So here are a few suggestions: If you have not yet done the "cavity" tutorial from the User Guide, I suggest that you do it, to confirm if ParaView is working properly. Copy the "system/controlDict" file to "system/controlDict.original". Then edit the file "system/controlDict" and remove everything below and including the line "functions". Save and close the file. Then run ParaView once again. If either one of these suggestions still give you an error, then there is something else going on that is causing the problems. Best regards, Bruno __________________ OpenFOAM: FAQ \| Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM

May 23, 2013, 04:22		#3
ngj Senior Member Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Copenhagen, Denmark Posts: 1,903 Rep Power: 37	Hi Amin, You are executing the tutorial in the root of the operating system, where you do not have permission to alter or add new files. Copy the entire tutorial folder to a location in your home directory, and you should be allowed to run the tutorials. Kind regards Niels

May 23, 2013, 06:40		#5
ngj Senior Member Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Copenhagen, Denmark Posts: 1,903 Rep Power: 37	Hi, Sorry, I was a bit quick in my answer, since I mostly focused on the "permission denied" part of the error. The tutorial changes some options in the file Code: /opt/openfoam220/etc/controlDict but since changes to this file are not permitted in the root directory, then you cannot execute the tutorial. I am not using 2.2.0 myself, so I do not know, what "codeStream" mentioned in the Allrun script does. One option is to (i) manually change the file /opt/openfoam220/etc/controlDict and then (ii) remove the relevant parts from the Allrun. Another option is to understand what codeStream does and remove it from the simulation. A third option is to enforce changes by the script by executing Code: sudo ./Allrun which will ask for your password and then you can potentially change everything in the root file system. If you are not familiar with the sudo command, please do read a bit about it, before you start using it. Kind regards Niels

May 23, 2013, 08:47		#7
Mirage12 Member Amin Join Date: May 2013 Posts: 76 Rep Power: 13	Thanks for your answer ! I tried to bluid the with blockMesh... but i received an Error. Code: --> FOAM FATAL IO ERROR: ill defined primitiveEntry starting at keyword '\|' on line 1 and ending at line 1028 file: /opt/openfoam220/etc/controlDict at line 1028. From function primitiveEntry::readEntry(const dictionary&, Istream&) in file db/dictionary/primitiveEntry/primitiveEntryIO.C at line 190 . I think haakon is right but i couldn't save the modification...because controlDict is in the file system..so how can save the change ? can you please explain why should i change the 0 to 1 ? Thanks a lot

May 23, 2013, 09:06		#8
haakon Senior Member Join Date: Dec 2011 Posts: 111 Rep Power: 20	First; you need to do the change as root. If you do not have that access, ask your system administrator to do the change for you (they are usually really nice and helpful). Second; you should change from 0 to 1 to allow OpenFOAM to build C++ code attached in the input files. See for example the code in tutorials/basic/potentialFoam/cylinder/system/controlDict as an example. It contain source code that needs to be compiled in order to work. The allowSystemOperations switch control this, if it 0 you are not allowed to build and execute source code from within the OpenFOAM input files.

May 28, 2013, 03:38		#15
Mirage12 Member Amin Join Date: May 2013 Posts: 76 Rep Power: 13	i am using ParaView-3.12.0-Linux-x86_64 and Ubuntu 12.04 and downloaded it from the website of ParaView http://www.paraview.org/paraview/resources/software.php Thanks for your support

May 29, 2013, 19:00		#18
wyldckat Retired Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,981 Blog Entries: 45 Rep Power: 128	Hi Amin, OK, I finally managed to figure it out. The problem is due to this in the "0/U" file: Code: left { type uniformFixedValue; uniformValue constant (1 0 0); } This is very different from what ParaView's internal ".foam" reader is expecting: Code: left { type uniformFixedValue; uniformValue uniform (1 0 0); } Problem is that this second form will not work with OpenFOAM. But the following should work for both OpenFOAM and ParaView: Code: left { type uniformFixedValue; uniformValue (1 0 0); } Keep in mind to edit the file "0.org/U" and perform all of the steps for executing once again! Best regards, Bruno __________________ OpenFOAM: FAQ \| Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Using createPatch and cyclicAMI in FOAM Extend to create periodicbox	manuc	OpenFOAM Running, Solving & CFD	1	April 12, 2022 12:36
create the file *.foam	phongstar	OpenFOAM	12	October 14, 2018 19:06
[GAMBIT] How to plot S pipe	mariam.sara	ANSYS Meshing & Geometry	36	November 7, 2013 16:22
[ANSYS Meshing] is it possible to create virtual edges on the blades	er_ijaz	ANSYS Meshing & Geometry	0	November 3, 2013 06:15
[DesignModeler] Design Modeller create surface	papis	ANSYS Meshing & Geometry	0	October 31, 2013 14:52