CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   error in parallel run (http://www.cfd-online.com/Forums/openfoam-solving/111153-error-parallel-run.html)

immortality December 29, 2012 07:38

error in parallel run
 
I run the case in serial scheme but when want to run in parallel it desn't perform.
thesis@thesis-X58A-UD7:~/Desktop/method_4_2_2(revised)-laminar.042$ decomposePar
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.1.0-0bc225064152
Exec : decomposePar
Date : Jan 29 2012
Time : 14:40:05
Host : "thesis-X58A-UD7"
PID : 6431
Case : /home/thesis/Desktop/method_4_2_2(revised)-laminar.042
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
Time = 0
Create mesh
Calculating distribution of cells
Selecting decompositionMethod simple
Finished decomposition in 0 s
Calculating original mesh data
Distributing cells to processors
Distributing faces to processors
Distributing points to processors
Constructing processor meshes
Processor 0
Number of cells = 3750
Number of faces shared with processor 1 = 30
Number of processor patches = 1
Number of processor faces = 30
Number of boundary faces = 7780
Processor 1
Number of cells = 3750
Number of faces shared with processor 0 = 30
Number of faces shared with processor 2 = 30
Number of processor patches = 2
Number of processor faces = 60
Number of boundary faces = 7750
Processor 2
Number of cells = 3750
Number of faces shared with processor 1 = 30
Number of faces shared with processor 3 = 30
Number of processor patches = 2
Number of processor faces = 60
Number of boundary faces = 7750
Processor 3
Number of cells = 3750
Number of faces shared with processor 2 = 30
Number of processor patches = 1
Number of processor faces = 30
Number of boundary faces = 7780
Number of processor faces = 90
Max number of cells = 3750 (0% above average 3750)
Max number of processor patches = 2 (33.3333% above average 1.5)
Max number of faces between processors = 60 (33.3333% above average 45)
 
 
--> FOAM FATAL IO ERROR:
Expected a '(' while reading VectorSpace<Form, Cmpt, nCmpt>, found on line 30 the doubleScalar 2.6
file: /home/thesis/Desktop/method_4_2_2(revised)-laminar.042/0/R::boundaryField::walls::value at line 30.
From function Istream::readBegin(const char*)
in file db/IOstreams/IOstreams/Istream.C at line 94.
FOAM exiting
thesis@thesis-X58A-UD7:~/Desktop/method_4_2_2(revised)-laminar.042$
 

wyldckat December 29, 2012 17:17

Greetings Ehsan,

OK... I think you need to read once again some instructions on how to get help: http://www.cfd-online.com/Forums/ope...-get-help.html

Because from what you've provided, I can only guess that you're triggering a bug that has already been fixed in either OpenFOAM 2.1.1 and/or 2.1.x.

The two lines after the big "FOAM FATAL IO ERROR:" line should pretty much be self-explanatory, if you have access to the file it's pointing to, namely the file "0/R".

Best regards,
Bruno

immortality December 30, 2012 11:32

hi
this is R folder.is there anything wrong with this?I only changed left patch to zeroGradient because this patch is changed between wall and surroundings.thank you for help.
Code:

| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volSymmTensorField;
location "0";
object R;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [ 0 2 -2 0 0 0 0 ];
internalField uniform ( 0 0 0 0 0 0 );
boundaryField
{
walls
{
type compressible::omegaWallFunction;
Cmu 0.09;
kappa 0.41;
E 9.8;
value uniform 2.6;
}
right
{
type kqRWallFunction;
value uniform ( 0 0 0 0 0 0 );
}
left
{
type zeroGradient;
}

empty
{
type empty;
}
}
 
// ************************************************************************* //


mkraposhin December 30, 2012 12:40

Is file R used in Your case? If this file is not used in Your case, then You must remove it

immortality December 31, 2012 03:38

hi.thanks.I used kOmegaSST and in walls it was set to kqrWallFunction.im not sure is this R related to that wall function?what folders are need to be in 0 folder for turbulency totally?
Thank you.

mkraposhin January 1, 2013 12:10

R - is Reynolds stress, predicted by k-omega sst model, it is not used in Your computation.

typical turbulent incompressible RAS case must have definition of initial and boundary conditions for next fields:
pressure - 0/p
velocity - 0/U
turbulent viscousity - 0/nut (for parametric RAS models)

Selected turbulence model introduces it's range of additional fields, for example:
kEpsilon - fields k and epsilon,
kOmega - fields k and omega,
SpalartAllmaras - fields k and nuTilde
RSTM - field R (reynolds stress tensor)
Choice of additional field is mutually exclusive

Selected additional fields determines contents of system/fvSchemes and system/fvSolution

immortality January 1, 2013 12:22

thanks.my case is compressible.so for kOmegaSST model I only need to k and omega folders?right?then I should delete other folders related to turbulancy like R.am I right?

mkraposhin January 1, 2013 13:35

Quote:

Originally Posted by immortality (Post 399650)
thanks.my case is compressible.so for kOmegaSST model I only need to k and omega folders?right?then I should delete other folders related to turbulancy like R.am I right?

Yes, You are right. for compressible case you need mut instead of nut, mut=rho*nut, temperature field T, alphat - turbulent enthalpy diffusion coefficient


All times are GMT -4. The time now is 03:38.