CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

MPI_ABORT running parallel simpleFoam

Register Blogs Community New Posts Updated Threads Search

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 15, 2017, 14:30
Default MPI_ABORT running parallel simpleFoam
  #1
New Member
 
Lluís M. Biscarri
Join Date: Nov 2011
Posts: 24
Rep Power: 14
biscarri is on a distinguished road
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
Attached Files
File Type: txt logSF.txt (6.1 KB, 8 views)
biscarri is offline   Reply With Quote

Old   June 16, 2017, 08:06
Default MPI_ABORT running parallel simpleFoam
  #2
New Member
 
Lluís M. Biscarri
Join Date: Nov 2011
Posts: 24
Rep Power: 14
biscarri is on a distinguished road
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
biscarri is offline   Reply With Quote

Old   June 16, 2017, 08:15
Default
  #3
Senior Member
 
floquation's Avatar
 
Kevin van As
Join Date: Sep 2014
Location: TU Delft, The Netherlands
Posts: 252
Rep Power: 20
floquation will become famous soon enough
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.
floquation is offline   Reply With Quote

Old   June 16, 2017, 11:05
Default
  #4
New Member
 
Lluís M. Biscarri
Join Date: Nov 2011
Posts: 24
Rep Power: 14
biscarri is on a distinguished road
Thank you very much for yur respnse, Kevin.

Please find enclosed the file log.simpleFoam resulting from
Code:
simpleFoam > log.simpleFoam 2>&1
I don't understand in this case the meaning of "FOAM FATAL ERROR: Could not find rho", after solving the first time step. I don't figure out what 'rho' has to do with simpleFoam, since I understand that NS equations are divided by 'rho' in OF.

I attach also file fvSolution with the convergence criteria for the diferent solvers. In this run simpleFoam is specified to complete 2000 timesteps.
Attached Files
File Type: txt log.simpleFoam.txt (3.0 KB, 4 views)
File Type: txt fvSolution.txt (2.5 KB, 2 views)
biscarri is offline   Reply With Quote

Old   June 16, 2017, 14:27
Default
  #5
Member
 
Joshua
Join Date: Dec 2016
Location: St. Louis, Missouri
Posts: 91
Rep Power: 9
Joshua14 is on a distinguished road
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
Joshua14 is offline   Reply With Quote

Old   June 16, 2017, 14:44
Default
  #6
New Member
 
Lluís M. Biscarri
Join Date: Nov 2011
Posts: 24
Rep Power: 14
biscarri is on a distinguished road
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.
Attached Files
File Type: txt forceCoeffs.txt (2.6 KB, 4 views)
File Type: txt transportProperties.txt (1.1 KB, 1 views)
biscarri is offline   Reply With Quote

Old   June 16, 2017, 15:06
Default
  #7
Member
 
Joshua
Join Date: Dec 2016
Location: St. Louis, Missouri
Posts: 91
Rep Power: 9
Joshua14 is on a distinguished road
What does your controlDict look like?
Joshua14 is offline   Reply With Quote

Old   June 16, 2017, 16:17
Default
  #8
New Member
 
Lluís M. Biscarri
Join Date: Nov 2011
Posts: 24
Rep Power: 14
biscarri is on a distinguished road
here it is controlDict file...
Attached Files
File Type: txt controlDict.txt (1.2 KB, 4 views)
biscarri is offline   Reply With Quote

Old   June 16, 2017, 16:31
Default
  #9
Member
 
Joshua
Join Date: Dec 2016
Location: St. Louis, Missouri
Posts: 91
Rep Power: 9
Joshua14 is on a distinguished road
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.
Joshua14 is offline   Reply With Quote

Old   June 17, 2017, 06:22
Default
  #10
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,932
Rep Power: 38
alexeym has a spectacular aura aboutalexeym has a spectacular aura about
Send a message via Skype™ to alexeym
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");
        ...
So this

Code:
...
pName               p; 
UName               U; 
rhoName             rhoInf; 
...
should be

Code:
p p;
U U;
rho rhoInf;
You can even remove p and U entries.

Also you can look at the header comment in $FOAM_SRC/functionObjects/forces/forces/forces.H, where parameters names are put into table.
alexeym is offline   Reply With Quote

Old   June 17, 2017, 08:49
Default
  #11
New Member
 
Lluís M. Biscarri
Join Date: Nov 2011
Posts: 24
Rep Power: 14
biscarri is on a distinguished road
Thank you very much Alexey, now simpleFOAM is processing forces properly.
biscarri is offline   Reply With Quote

Reply


Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


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 03:15
Problem running movingCylinders case in parallel with foam-extend-3.1 mhkenergy OpenFOAM Running, Solving & CFD 5 March 3, 2017 05:20
Running parallel case after parallel meshing with snappyHexMesh? Adam Persson OpenFOAM Running, Solving & CFD 0 August 31, 2015 22:04
Problem in Running OpenFoam in Parallel himanshu28 OpenFOAM Running, Solving & CFD 1 July 11, 2013 09:19
parallel running - error while loading shared libraries: seami OpenFOAM Installation 1 December 9, 2011 04:39


All times are GMT -4. The time now is 04:32.