|
[Sponsors] |
December 29, 2012, 07:38 |
error in parallel run
|
#1 |
Senior Member
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,208
Rep Power: 27 |
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$ |
|
December 29, 2012, 17:17 |
|
#2 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,980
Blog Entries: 45
Rep Power: 128 |
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
__________________
|
|
December 30, 2012, 11:32 |
|
#3 |
Senior Member
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,208
Rep Power: 27 |
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; } } // ************************************************************************* // |
|
December 30, 2012, 12:40 |
|
#4 |
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 355
Rep Power: 21 |
Is file R used in Your case? If this file is not used in Your case, then You must remove it
|
|
December 31, 2012, 03:38 |
|
#5 |
Senior Member
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,208
Rep Power: 27 |
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. |
|
January 1, 2013, 12:10 |
|
#6 |
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 355
Rep Power: 21 |
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 |
|
January 1, 2013, 12:22 |
|
#7 |
Senior Member
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,208
Rep Power: 27 |
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?
|
|
January 1, 2013, 13:35 |
|
#8 |
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 355
Rep Power: 21 |
Yes, You are right. for compressible case you need mut instead of nut, mut=rho*nut, temperature field T, alphat - turbulent enthalpy diffusion coefficient
|
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Case running in serial, but Parallel run gives error | atmcfd | OpenFOAM Running, Solving & CFD | 18 | March 26, 2016 12:40 |
Parallel Run on dynamically mounted partition | braennstroem | OpenFOAM Running, Solving & CFD | 14 | October 5, 2010 14:43 |
Unable to run OF in parallel on a multiple-node cluster | quartzian | OpenFOAM | 3 | November 24, 2009 13:37 |
serial run fine, but parallel run diverged | phsieh2005 | OpenFOAM Running, Solving & CFD | 2 | October 6, 2009 08:33 |
Run in parallel a 2mesh case | cosimobianchini | OpenFOAM Running, Solving & CFD | 2 | January 11, 2007 06:33 |