|
[Sponsors] |
June 10, 2015, 15:27 |
own turbulence model not working in parallel
|
#1 |
Member
Aditya
Join Date: Nov 2014
Posts: 35
Rep Power: 11 |
Hi everyone,
I have modified and implemented a new turbulence model in openfoam and compiled the library succesfully. I have also used the turbulence model without any problem on a single processor. But when i try to decompose the domain and run it in parallel, I get the follwing error HTML Code:
Processor 1 Number of cells = 6473 Number of faces shared with processor 0 = 100 Number of faces shared with processor 3 = 67 Number of processor patches = 2 Number of processor faces = 167 Number of boundary faces = 13109 --> FOAM Warning : From function dlOpen(const fileName&, const bool) in file POSIX.C at line 1179 dlopen error : /home/aditya/OpenFOAM/aditya-2.3.0/platforms/linux64GccDPOpt/lib/libmyIncompressibleRASTransitionModel.so: undefined symbol: _ZTIN4Foam14incompressible8RASModelE --> FOAM Warning : From function dlLibraryTable::open(const fileName&, const bool) in file db/dynamicLibrary/dlLibraryTable/dlLibraryTable.C at line 99 could not load "libmyIncompressibleRASTransitionModel.so" Thanks in advance!! |
|
June 11, 2015, 05:42 |
|
#2 |
Senior Member
Yogesh Bapat
Join Date: Oct 2010
Posts: 102
Rep Power: 15 |
Hello,
Add line libs ("libmyIncompressibleRASTransitionModel.so"); to controlDict file so that decomposepar is able to load your library. Regards, -Yogesh |
|
June 11, 2015, 14:01 |
|
#3 |
New Member
Aditya D S N
Join Date: Oct 2011
Posts: 5
Rep Power: 14 |
Hi,
I do have that line in my control dict. It works perfectly when i run the case in serial but when i try to run it in parallel it gives me the error. when i use the decomposePar command, i get the above mentioned error. |
|
June 17, 2015, 15:34 |
|
#4 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,974
Blog Entries: 45
Rep Power: 128 |
Quick answer: Change the line:
Code:
libs ("libmyIncompressibleRASTransitionModel.so"); Code:
libs ( "libmyIncompressibleRASTransitionModel.so" "libincompressibleRASModels.so" ); Code:
undefined symbol: _ZTIN4Foam14incompressible8RASModelE |
|
June 17, 2015, 16:52 |
|
#5 |
Member
Aditya
Join Date: Nov 2014
Posts: 35
Rep Power: 11 |
Thank you so much wyldkat. That worked!!
But I'm a little curious because this worked HTML Code:
libs ("libincompressibleRASModels.so" "libmyIncompressibleRASTransitionModel.so" "libfindroot.so" ); HTML Code:
libs ( "libmyIncompressibleRASTransitionModel.so" "libfindroot.so" "libincompressibleRASModels.so" ); Regards, Aditya |
|
June 21, 2015, 15:58 |
|
#6 | |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,974
Blog Entries: 45
Rep Power: 128 |
Quote:
Code:
undefined symbol: _ZTIN4Foam14incompressible8RASModelE Unfortunately I was in a hurry and didn't think about the loading priority, namely that we must first load the library that has the symbol we need, so that we can load our own library. |
||
January 12, 2016, 19:12 |
Error message after runing paraFoam
|
#7 |
New Member
adhi makayasa
Join Date: Apr 2015
Posts: 20
Rep Power: 11 |
Hi all,
after running paraFoam, in the terminal to get a message like this. From function dlOpen(const fileName&, const bool) in file POSIX.C at line 1179 dlopen error : /home/yasa/OpenFOAM/yasa-2.3.0/platforms/linuxGccDPOpt/lib/libmyIncompressibleRASModels.so: undefined symbol: _ZTIN4Foam14incompressible8RASModelE FOAM Warning : From function dlLibraryTable:pen(const fileName&, const bool) in file db/dynamicLibrary/dlLibraryTable/dlLibraryTable.C at line 99 could not load "libmyIncompressibleRASModels.so" How to fix it? Please help, this is my final assignment |
|
February 24, 2016, 21:46 |
|
#8 |
New Member
Sami
Join Date: Dec 2014
Posts: 1
Rep Power: 0 |
Hello guys,
I got same message but after I run the solver "pisoFoam" .... the message was: pisoFoam: symbol lookup error: /.../..../OpenFOAM/......-2.1.0/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so: undefined symbol: _ZTIN4Foam14incompressible8RASModelE I do not know how to solve!!!!!! any idea ?? Thanks a lot .. Sami |
|
February 29, 2016, 11:08 |
|
#9 |
Member
Peter
Join Date: Nov 2015
Location: Hamburg, Germany
Posts: 57
Rep Power: 10 |
Dear Sami,
seems as if the same library is not linked. Can you please post your controlDict-file? Peter |
|
April 27, 2020, 07:33 |
|
#10 | |
Senior Member
Join Date: Dec 2019
Location: Cologne, Germany
Posts: 355
Rep Power: 8 |
Quote:
after you add it you need to compile once again. |
||
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Parallel running of 3D multiphase turbulence model (unknown problem!!) | MOHAMMAD67 | OpenFOAM Running, Solving & CFD | 7 | November 23, 2015 10:53 |
Turbulence Model - Linking Issues? | AA29 | OpenFOAM Programming & Development | 3 | June 20, 2014 15:21 |
Compressible turbulence model issues | 351Cleveland | OpenFOAM | 5 | October 24, 2013 15:41 |
new turbulence model in Fluent | C.C | FLUENT | 0 | August 29, 2013 10:44 |
Sinclair Model + secondary turbulence | Yi | FLUENT | 0 | October 26, 2001 13:37 |