|
[Sponsors] |
June 15, 2017, 15:30 |
MPI_ABORT running parallel simpleFoam
|
#1 |
New Member
Lluís M. Biscarri
Join Date: Nov 2011
Posts: 24
Rep Power: 15 |
Hi,
I run a model in parallel with simpleFOAM, that worked OK with OF previous version, and now when running with OF3.0.0 gives and MPI_ABORT error. Please find enclosed log file. Thanks for any help, advice. Lluis |
|
June 16, 2017, 09:06 |
MPI_ABORT running parallel simpleFoam
|
#2 |
New Member
Lluís M. Biscarri
Join Date: Nov 2011
Posts: 24
Rep Power: 15 |
In the parallel run the MPI_ABORT error is produced after simpleFoam completes the first time iteration.
I have tried to run the case in serial and simpleFoam completes the first time step but does not continue iterating (contrlDict file specifies to run 2000 time steps) and does not create postPrcessing folder with results. Then the problem seems to have no relation with running the case in parallel. Any suggestion? Thank U |
|
June 16, 2017, 09:15 |
|
#3 |
Senior Member
Kevin van As
Join Date: Sep 2014
Location: TU Delft, The Netherlands
Posts: 252
Rep Power: 21 |
No one will be able to help you if you only post the STDOUT stream. The useful information is usually contained in the STDERR stream.
When you redirect your solver output to a file, please also redirect the error to it: Code:
solverName >log 2>&1 Although, I do notice that your solver seems to only care about achieving a residual of 0.1 for k. What convergence criterion did you specify? Then I see that kmin is negative. Something is probably going wrong right there. |
|
June 16, 2017, 12:05 |
|
#4 |
New Member
Lluís M. Biscarri
Join Date: Nov 2011
Posts: 24
Rep Power: 15 |
Thank you very much for yur respnse, Kevin.
Please find enclosed the file log.simpleFoam resulting from Code:
simpleFoam > log.simpleFoam 2>&1 I attach also file fvSolution with the convergence criteria for the diferent solvers. In this run simpleFoam is specified to complete 2000 timesteps. |
|
June 16, 2017, 15:27 |
|
#5 |
Member
Joshua
Join Date: Dec 2016
Location: St. Louis, Missouri
Posts: 91
Rep Power: 10 |
The reason your simulation crashed is that rho does not seem to be defined for your function object forces.
--> FOAM FATAL ERROR: Could not find rho From function void Foam::functionObjects::forces::initialise() in file forces/forces.C at line 196. FOAM exiting Joshua |
|
June 16, 2017, 15:44 |
|
#6 |
New Member
Lluís M. Biscarri
Join Date: Nov 2011
Posts: 24
Rep Power: 15 |
Thanks for the comment, Joshua.
The folder constant contains the file transportProperties, where rho and nu are defined. The forceCoeffs file in the system folder contains the definition of rhoName and rhoInf for postprocessing purposes.. Please find those files attached. |
|
June 16, 2017, 16:06 |
|
#7 |
Member
Joshua
Join Date: Dec 2016
Location: St. Louis, Missouri
Posts: 91
Rep Power: 10 |
What does your controlDict look like?
|
|
June 16, 2017, 17:17 |
|
#8 |
New Member
Lluís M. Biscarri
Join Date: Nov 2011
Posts: 24
Rep Power: 15 |
here it is controlDict file...
|
|
June 16, 2017, 17:31 |
|
#9 |
Member
Joshua
Join Date: Dec 2016
Location: St. Louis, Missouri
Posts: 91
Rep Power: 10 |
Everything looks like it is defined right. I am not sure why it is erroring out then. It is hung up on the postProcessing step tho. Hence the forces.C file.
|
|
June 17, 2017, 07:22 |
|
#10 |
Senior Member
|
Hi all,
@biscarri If you look into $FOAM_SRC/functionObjects/forces/forces/forces.C read method: Code:
... // Optional entries U and p pName_ = dict.lookupOrDefault<word>("p", "p"); UName_ = dict.lookupOrDefault<word>("U", "U"); rhoName_ = dict.lookupOrDefault<word>("rho", "rho"); ... Code:
... pName p; UName U; rhoName rhoInf; ... Code:
p p; U U; rho rhoInf; Also you can look at the header comment in $FOAM_SRC/functionObjects/forces/forces/forces.H, where parameters names are put into table. |
|
June 17, 2017, 09:49 |
|
#11 |
New Member
Lluís M. Biscarri
Join Date: Nov 2011
Posts: 24
Rep Power: 15 |
Thank you very much Alexey, now simpleFOAM is processing forces properly.
|
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
OF 2.0.1 parallel running problems | moser_r | OpenFOAM Running, Solving & CFD | 9 | July 27, 2022 04:15 |
Problem running movingCylinders case in parallel with foam-extend-3.1 | mhkenergy | OpenFOAM Running, Solving & CFD | 5 | March 3, 2017 06:20 |
Running parallel case after parallel meshing with snappyHexMesh? | Adam Persson | OpenFOAM Running, Solving & CFD | 0 | August 31, 2015 23:04 |
Problem in Running OpenFoam in Parallel | himanshu28 | OpenFOAM Running, Solving & CFD | 1 | July 11, 2013 10:19 |
parallel running - error while loading shared libraries: | seami | OpenFOAM Installation | 1 | December 9, 2011 05:39 |