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

LEMOS InflowGenerator

Register Blogs Community New Posts Updated Threads Search

Like Tree25Likes

Reply
Page 3 of 6 12 3 45 Last »
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 28, 2014, 07:58
Default
  #41
Senior Member
 
Hannes Kröger
Join Date: Mar 2009
Location: Rostock, Germany
Posts: 123
Rep Power: 18
hannes is on a distinguished road
Dear openfoammaofnepo,

the integral length scale you prescribed is 35% of the width of the inlet ring. It seems ok, perhaps a bit too high. I would generally expect something like one order of magnitude less than the characteristic flow length scale.

Note that the prescribed length scale is connected to the size of the generated spots. If it gets too small into the order of the face size on your patch, the inner velocity structure of the spots can't be resolved any more. And also since the whole patch area shall be covered with (overlapping) spots, their number may grow to a very high value, when the length scale gets very small.

Regarding the vorton list in the U file: it seems the paraFoam reader gets confused by it. I don't use this but the internal reader of paraview instead. It works fine with this.

The vorton list is not treated during reconstruction from parallel run. I currently work on a new version of the inflow generator BC and this problem is fixed in it. But this version is not ready for release yet.
hannes is offline   Reply With Quote

Old   November 28, 2014, 08:33
Default
  #42
Senior Member
 
Join Date: Jan 2013
Posts: 372
Rep Power: 14
openfoammaofnepo is on a distinguished road
Dear Hannes,

Thank you for your reply. About the paraFOAm, actually I did not use that either. I use the paraview which is directly download from the official website. Could you tell which is 'internal reader'? Thank you.

About the "ind_", could you please give me some hints about fixing this problem? Since I will frequently resume the simulation, it will be not convenient to fix ind_ number each time in the reconstructed data set. Thank you very much.



Quote:
Originally Posted by hannes View Post
Dear openfoammaofnepo,

the integral length scale you prescribed is 35% of the width of the inlet ring. It seems ok, perhaps a bit too high. I would generally expect something like one order of magnitude less than the characteristic flow length scale.

Note that the prescribed length scale is connected to the size of the generated spots. If it gets too small into the order of the face size on your patch, the inner velocity structure of the spots can't be resolved any more. And also since the whole patch area shall be covered with (overlapping) spots, their number may grow to a very high value, when the length scale gets very small.

Regarding the vorton list in the U file: it seems the paraFoam reader gets confused by it. I don't use this but the internal reader of paraview instead. It works fine with this.

The vorton list is not treated during reconstruction from parallel run. I currently work on a new version of the inflow generator BC and this problem is fixed in it. But this version is not ready for release yet.
openfoammaofnepo is offline   Reply With Quote

Old   December 15, 2014, 08:30
Default
  #43
Member
 
Join Date: Apr 2011
Posts: 57
Rep Power: 15
amanbearpig is on a distinguished road
Dear openfoammaofnepo, Hannes, or anyone else who could shed some light on this for me:

I have installed the LEMOS Inflow Generator and am attempting to use it for flow over a flat plate to test it out. I'm doing LES, and have put a generic boundary layer profile for the velocity at the inlet, and just to test it out, I put a RField of (1 0 0 1 0 1);. Obviously this is not correct, but I am merely trying to test it out and see what results I get. (Just as a note, I have also tested using an RField calculated from a RANS run, with the same results, in case the lack of any velocity perturbations was due to the generic RField). I then run pimpleFoam, and in the log file I see that the Inflow Generator is enabled and running, as it prints out (as an example from a case I just ran):
Code:
PIMPLE: iteration 1
[0] Starting inflgen, time = 116 s
[0] The number of vortons is 773
[0] Finishing inflgen, time = 117 s
However, when I then run decomposePar and foamToVTK to take a look at the resulting field, I don't see any kind of change in the velocity field (See attached image). It looks identical to the field prior to implementing the Inflow Generator. Is there something I need to look for or any guidance on how to make sure the Inflow Generator is properly working, or (more likely) to ensure I am not making any obvious mistakes? Thank you very much!
Attached Images
File Type: jpg NoVortons.jpg (13.8 KB, 77 views)
amanbearpig is offline   Reply With Quote

Old   December 15, 2014, 08:33
Default
  #44
Senior Member
 
Hannes Kröger
Join Date: Mar 2009
Location: Rostock, Germany
Posts: 123
Rep Power: 18
hannes is on a distinguished road
Dear armanbearpig,

can you share your case?

Regards, Hannes
hannes is offline   Reply With Quote

Old   December 15, 2014, 08:43
Default
  #45
Member
 
Join Date: Apr 2011
Posts: 57
Rep Power: 15
amanbearpig is on a distinguished road
Thank you for the speedy reply Hannes, . I can share it, however it is a bit too big to attach here I believe. Should I just attach a particular file or two?
amanbearpig is offline   Reply With Quote

Old   December 15, 2014, 08:47
Default
  #46
Senior Member
 
Hannes Kröger
Join Date: Mar 2009
Location: Rostock, Germany
Posts: 123
Rep Power: 18
hannes is on a distinguished road
I'd like to be able to start it.
Maybe via dropbox? You can send me the link via a private message.
hannes is offline   Reply With Quote

Old   December 16, 2014, 01:36
Default
  #47
Senior Member
 
Hannes Kröger
Join Date: Mar 2009
Location: Rostock, Germany
Posts: 123
Rep Power: 18
hannes is on a distinguished road
Dear amanbearpig,

when you look at velocity magnitude after the first few timesteps it looks indeed like there are no fluctuations generated (first image). Although when you take a look at U_Z, you see that they are there but very small.
At a later timestep, the fluctuations reach their full magnitude (third image, haven't checked, if the values are reasonably prescribed here).

The generated raw fluctuations have an amplitude that depends on the length scale and the spot internal velocity distribution. For reproduction of precribed Reynolds stresses, the raw fluctuation need to be normalized by this a priori unknown factor. In the current implementation, the scaling factor is determined by some online adaption of the statistics. Thus it takes a number of timesteps until the fluctuations are right.

Currently, we have a heavily improved version of the inflow generator, which is not only capable of generating divergence-free fluctuations with almost arbitrary anisotropy but also determined the scaling factor in an analytical way in advance, so this nasty adaption time has been removed.
But before releasing it, we want to check it and publish results first...

Regards, Hannes
Attached Images
File Type: jpg Auswahl_068.jpg (20.0 KB, 136 views)
File Type: jpg Auswahl_069.jpg (30.8 KB, 163 views)
File Type: jpg Auswahl_070.jpg (34.7 KB, 152 views)
amanbearpig, PonchO and tiam like this.
hannes is offline   Reply With Quote

Old   December 17, 2014, 07:31
Default
  #48
Member
 
Join Date: Apr 2011
Posts: 57
Rep Power: 15
amanbearpig is on a distinguished road
Hi Hannes,

Thank you very much! That makes sense to me now - I didn't realize it took some time for the fluctuations to reach the correct magnitude. I've tested it here as well and if I let it run for awhile the fluctuations do increase in magnitude so that they are noticeable. Thank you again for your very timely help, and I look forward to seeing the forthcoming iterations of the Inflow Generator!
amanbearpig is offline   Reply With Quote

Old   March 20, 2015, 07:03
Default
  #49
Senior Member
 
Join Date: Jan 2013
Posts: 372
Rep Power: 14
openfoammaofnepo is on a distinguished road
Hi All,

For this turbulent boundary condition, if the CFL number close to the inlet is relatively large, will this have any effects on mimicking the inlet turbulence using the current boundary conditions? Since I found that near the inlet the CFL number is always large caused by the high inlet bulk velocity there.

Thank you for your help.

OFFO
openfoammaofnepo is offline   Reply With Quote

Old   March 25, 2015, 13:50
Default
  #50
Member
 
Daniel
Join Date: Jun 2014
Posts: 60
Rep Power: 11
Dan1788 is on a distinguished road
Hello,

I had a question. Since RField is the reynolds stress field and the turbulent intensity is sqrt(normal reynolds stress), should the value of RField (0.01 0 0 0.01 0 0.01) be reasonable ? That ways the intensity is 10% in all directions.

Is my thinking correct ?
Dan1788 is offline   Reply With Quote

Old   April 11, 2015, 05:17
Default Problem in installing LEMOS-Rostock-2.3.x in OF 2.3.1
  #51
Senior Member
 
cfdonline2mohsen's Avatar
 
Mohsen KiaMansouri
Join Date: Jan 2010
Location: CFD Lab
Posts: 118
Rep Power: 16
cfdonline2mohsen is on a distinguished road
Dear Foamers,
I want to install LEMOS-Rostock-2.3.x in OF 2.3.1:
https://github.com/LEMOS-Rostock/LEMOS-2.3.x
I took the following steps as in the README.md file:

  1. move the Folder "LEMOS-2.3.x" into $FOAM_SRC
  2. add the following line to your ~/.bashrc after ". ~/OpenFOAM/OpenFOAM-2.3.x/etc/bashrc": . $FOAM_SRC/LEMOS-2.3.x/bashrc
  3. parse your ~/.bashrc or open a new terminal
  4. Execute applyPatches to install patches in $FOAM_SRC folder
  5. Execute $LEMOSEXT/Allwmake to build the library and executables
But in the 5th step, I have encountered the following error messages:

Code:
vahid@ubuntu:/opt/openfoam231/src/LEMOS-2.3.x-master$ ./Allwmake
  + wmake libso libLEMOS-2.3.x
  '/opt/openfoam231/platforms/linux64GccDPOpt/lib/libLEMOS-2.3.x.so' is up to date.
  + cd applications
  + wmake all solvers
  make[1]: Entering directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/solvers/basic'
  make[2]: Entering directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/solvers/basic/PODSolver'
  SOURCE=PODSolver.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/libLEMOS-2.3.x/lnInclude -I/opt/openfoam231/src/finiteVolume/lnInclude  -IlnInclude -I. -I/opt/openfoam231/src/OpenFOAM/lnInclude -I/opt/openfoam231/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/PODSolver.o
  PODSolver.C:35:20: fatal error: PODODE.H: No such file or directory
   #include "PODODE.H"
                      ^
  compilation terminated.
  make[2]: *** [Make/linux64GccDPOpt/PODSolver.o] Error 1
  make[2]: Target `/opt/openfoam231/platforms/linux64GccDPOpt/bin/PODSolver' not remade because of errors.
  make[2]: Leaving directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/solvers/basic/PODSolver'
  make[1]: *** [PODSolver] Error 2
  make[1]: Target `application' not remade because of errors.
  make[1]: Leaving directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/solvers/basic'
  make: *** [basic] Error 2
  make: Target `application' not remade because of errors.
  + cd applications
  + wmake all utilities
  make[1]: Entering directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing'
  make[2]: Entering directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/POD'
  make[3]: Entering directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/POD/scalarSnapshots'
  SOURCE=scalarSnapshots.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/libLEMOS-2.3.x/lnInclude -I/opt/openfoam231/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam231/src/OpenFOAM/lnInclude -I/opt/openfoam231/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/scalarSnapshots.o
  scalarSnapshots.C:37:33: fatal error: PODOrthoNormalBases.H: No such file or directory
   #include "PODOrthoNormalBases.H"
                                   ^
  compilation terminated.
  make[3]: *** [Make/linux64GccDPOpt/scalarSnapshots.o] Error 1
  make[3]: Target `/opt/openfoam231/platforms/linux64GccDPOpt/bin/scalarSnapshots' not remade because of errors.
  make[3]: Leaving directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/POD/scalarSnapshots'
  make[2]: *** [scalarSnapshots] Error 2
  make[3]: Entering directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/POD/vectorSnapshots'
  SOURCE=vectorSnapshots.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/libLEMOS-2.3.x/lnInclude -I/opt/openfoam231/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam231/src/OpenFOAM/lnInclude -I/opt/openfoam231/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/vectorSnapshots.o
  vectorSnapshots.C:37:33: fatal error: PODOrthoNormalBases.H: No such file or directory
   #include "PODOrthoNormalBases.H"
                                   ^
  compilation terminated.
  make[3]: *** [Make/linux64GccDPOpt/vectorSnapshots.o] Error 1
  make[3]: Target `/opt/openfoam231/platforms/linux64GccDPOpt/bin/vectorSnapshots' not remade because of errors.
  make[3]: Leaving directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/POD/vectorSnapshots'
  make[2]: *** [vectorSnapshots] Error 2
  make[2]: Target `application' not remade because of errors.
  make[2]: Leaving directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/POD'
  make[1]: *** [POD] Error 2
  make[2]: Entering directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/miscellaneous'
  make[3]: Entering directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/miscellaneous/postChannelExt'
  SOURCE=postChannelExt.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/opt/openfoam231/src/meshTools/lnInclude -I/opt/openfoam231/src/finiteVolume/lnInclude -I/opt/openfoam231/src/sampling/lnInclude -I/OpenFOAM/primitives/Triple -IlnInclude -I. -I/opt/openfoam231/src/OpenFOAM/lnInclude -I/opt/openfoam231/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/postChannelExt.o
  postChannelExt.C:38:20: fatal error: Triple.H: No such file or directory
   #include "Triple.H"
                      ^
  compilation terminated.
  make[3]: *** [Make/linux64GccDPOpt/postChannelExt.o] Error 1
  make[3]: Target `/opt/openfoam231/platforms/linux64GccDPOpt/bin/postChannelExt' not remade because of errors.
  make[3]: Leaving directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/miscellaneous/postChannelExt'
  make[2]: *** [postChannelExt] Error 2
  make[2]: Target `application' not remade because of errors.
  make[2]: Leaving directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/miscellaneous'
  make[1]: *** [miscellaneous] Error 2
  make[2]: Entering directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/velocityField'
  make[3]: Entering directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/velocityField/LambdaCI'
  make[3]: `/opt/openfoam231/platforms/linux64GccDPOpt/bin/LambdaCI' is up to date.
  make[3]: Leaving directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/velocityField/LambdaCI'
  make[2]: Leaving directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/velocityField'
  make[1]: Target `application' not remade because of errors.
  make[1]: Leaving directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing'
  make: *** [postProcessing] Error 2
  make: Target `application' not remade because of errors.
Any help would be much appreciated.
__________________
“If you have an apple and I have an apple and we exchange these apples then you and I will still each have one apple. But if you have an idea and I have an idea and we exchange these ideas, then each of us will have two ideas.”
cfdonline2mohsen is offline   Reply With Quote

Old   April 11, 2015, 07:07
Default
  #52
Senior Member
 
cfdonline2mohsen's Avatar
 
Mohsen KiaMansouri
Join Date: Jan 2010
Location: CFD Lab
Posts: 118
Rep Power: 16
cfdonline2mohsen is on a distinguished road
Quote:
Originally Posted by cfdonline2mohsen View Post
Dear Foamers,
I want to install LEMOS-Rostock-2.3.x in OF 2.3.1:
https://github.com/LEMOS-Rostock/LEMOS-2.3.x
I took the following steps as in the README.md file:

  1. move the Folder "LEMOS-2.3.x" into $FOAM_SRC
  2. add the following line to your ~/.bashrc after ". ~/OpenFOAM/OpenFOAM-2.3.x/etc/bashrc": . $FOAM_SRC/LEMOS-2.3.x/bashrc
  3. parse your ~/.bashrc or open a new terminal
  4. Execute applyPatches to install patches in $FOAM_SRC folder
  5. Execute $LEMOSEXT/Allwmake to build the library and executables
But in the 5th step, I have encountered the following error messages:

Code:
vahid@ubuntu:/opt/openfoam231/src/LEMOS-2.3.x-master$ ./Allwmake
  + wmake libso libLEMOS-2.3.x
  '/opt/openfoam231/platforms/linux64GccDPOpt/lib/libLEMOS-2.3.x.so' is up to date.
  + cd applications
  + wmake all solvers
  make[1]: Entering directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/solvers/basic'
  make[2]: Entering directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/solvers/basic/PODSolver'
  SOURCE=PODSolver.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/libLEMOS-2.3.x/lnInclude -I/opt/openfoam231/src/finiteVolume/lnInclude  -IlnInclude -I. -I/opt/openfoam231/src/OpenFOAM/lnInclude -I/opt/openfoam231/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/PODSolver.o
  PODSolver.C:35:20: fatal error: PODODE.H: No such file or directory
   #include "PODODE.H"
                      ^
  compilation terminated.
  make[2]: *** [Make/linux64GccDPOpt/PODSolver.o] Error 1
  make[2]: Target `/opt/openfoam231/platforms/linux64GccDPOpt/bin/PODSolver' not remade because of errors.
  make[2]: Leaving directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/solvers/basic/PODSolver'
  make[1]: *** [PODSolver] Error 2
  make[1]: Target `application' not remade because of errors.
  make[1]: Leaving directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/solvers/basic'
  make: *** [basic] Error 2
  make: Target `application' not remade because of errors.
  + cd applications
  + wmake all utilities
  make[1]: Entering directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing'
  make[2]: Entering directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/POD'
  make[3]: Entering directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/POD/scalarSnapshots'
  SOURCE=scalarSnapshots.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/libLEMOS-2.3.x/lnInclude -I/opt/openfoam231/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam231/src/OpenFOAM/lnInclude -I/opt/openfoam231/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/scalarSnapshots.o
  scalarSnapshots.C:37:33: fatal error: PODOrthoNormalBases.H: No such file or directory
   #include "PODOrthoNormalBases.H"
                                   ^
  compilation terminated.
  make[3]: *** [Make/linux64GccDPOpt/scalarSnapshots.o] Error 1
  make[3]: Target `/opt/openfoam231/platforms/linux64GccDPOpt/bin/scalarSnapshots' not remade because of errors.
  make[3]: Leaving directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/POD/scalarSnapshots'
  make[2]: *** [scalarSnapshots] Error 2
  make[3]: Entering directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/POD/vectorSnapshots'
  SOURCE=vectorSnapshots.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/libLEMOS-2.3.x/lnInclude -I/opt/openfoam231/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam231/src/OpenFOAM/lnInclude -I/opt/openfoam231/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/vectorSnapshots.o
  vectorSnapshots.C:37:33: fatal error: PODOrthoNormalBases.H: No such file or directory
   #include "PODOrthoNormalBases.H"
                                   ^
  compilation terminated.
  make[3]: *** [Make/linux64GccDPOpt/vectorSnapshots.o] Error 1
  make[3]: Target `/opt/openfoam231/platforms/linux64GccDPOpt/bin/vectorSnapshots' not remade because of errors.
  make[3]: Leaving directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/POD/vectorSnapshots'
  make[2]: *** [vectorSnapshots] Error 2
  make[2]: Target `application' not remade because of errors.
  make[2]: Leaving directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/POD'
  make[1]: *** [POD] Error 2
  make[2]: Entering directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/miscellaneous'
  make[3]: Entering directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/miscellaneous/postChannelExt'
  SOURCE=postChannelExt.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/opt/openfoam231/src/meshTools/lnInclude -I/opt/openfoam231/src/finiteVolume/lnInclude -I/opt/openfoam231/src/sampling/lnInclude -I/OpenFOAM/primitives/Triple -IlnInclude -I. -I/opt/openfoam231/src/OpenFOAM/lnInclude -I/opt/openfoam231/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/postChannelExt.o
  postChannelExt.C:38:20: fatal error: Triple.H: No such file or directory
   #include "Triple.H"
                      ^
  compilation terminated.
  make[3]: *** [Make/linux64GccDPOpt/postChannelExt.o] Error 1
  make[3]: Target `/opt/openfoam231/platforms/linux64GccDPOpt/bin/postChannelExt' not remade because of errors.
  make[3]: Leaving directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/miscellaneous/postChannelExt'
  make[2]: *** [postChannelExt] Error 2
  make[2]: Target `application' not remade because of errors.
  make[2]: Leaving directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/miscellaneous'
  make[1]: *** [miscellaneous] Error 2
  make[2]: Entering directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/velocityField'
  make[3]: Entering directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/velocityField/LambdaCI'
  make[3]: `/opt/openfoam231/platforms/linux64GccDPOpt/bin/LambdaCI' is up to date.
  make[3]: Leaving directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/velocityField/LambdaCI'
  make[2]: Leaving directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing/velocityField'
  make[1]: Target `application' not remade because of errors.
  make[1]: Leaving directory `/opt/openfoam231/src/LEMOS-2.3.x-master/applications/utilities/postProcessing'
  make: *** [postProcessing] Error 2
  make: Target `application' not remade because of errors.
Any help would be much appreciated.
Sorry for spamming the thread.
I have found my mistake.
The name of the folder must be LEMOS-2.3.x NOT LEMOS-2.3.x-master
__________________
“If you have an apple and I have an apple and we exchange these apples then you and I will still each have one apple. But if you have an idea and I have an idea and we exchange these ideas, then each of us will have two ideas.”
cfdonline2mohsen is offline   Reply With Quote

Old   June 13, 2015, 11:18
Default
  #53
Senior Member
 
Syavash Asgari
Join Date: Apr 2010
Posts: 473
Rep Power: 18
syavash is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
Quick answer:
If you're looking for something more, please be a bit more specific

Dear Bruno,

Do you know how to implement a non-uniform velocity B.C. (e.g. a logarithmic profile) in LeMOS inflow turbulence generator?! Can you give a brief example?

Thanks
syavash is offline   Reply With Quote

Old   June 13, 2015, 13:24
Default
  #54
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quote:
Originally Posted by syavash View Post
Dear Bruno,

Do you know how to implement a non-uniform velocity B.C. (e.g. a logarithmic profile) in LeMOS inflow turbulence generator?! Can you give a brief example?

Thanks
Quick answer: Don't ask me. I never used LEMOS
I merely pointed out on that post you quoted where information about it could be found. And sadly I don't have time to go exploring it.
wyldckat is offline   Reply With Quote

Old   June 13, 2015, 14:41
Default
  #55
Senior Member
 
Syavash Asgari
Join Date: Apr 2010
Posts: 473
Rep Power: 18
syavash is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
Quick answer: Don't ask me. I never used LEMOS
I merely pointed out on that post you quoted where information about it could be found. And sadly I don't have time to go exploring it.
Thanks anyway,
Regards
syavash is offline   Reply With Quote

Old   June 14, 2015, 12:32
Default
  #56
Senior Member
 
Syavash Asgari
Join Date: Apr 2010
Posts: 473
Rep Power: 18
syavash is on a distinguished road
All rights, I have gone through all the threads about inflow generator, but I could not find any person who could/have implement a non-uniform velocity boundary condition in LeMOS inflow generator. Can you please elaborate this a little further??!!! A brief example would be highly appreciated. I do not have any idea how to do this myself.

Regards
syavash is offline   Reply With Quote

Old   June 14, 2015, 13:18
Default
  #57
Senior Member
 
Hannes Kröger
Join Date: Mar 2009
Location: Rostock, Germany
Posts: 123
Rep Power: 18
hannes is on a distinguished road
Dear syavash,

all required fields for the inflowGenerator-BC can be specified "uniform" or "nonuniform" in space but only steady in time. Unfortunately, there is no straightforward and comfortable way in OpenFOAM to specify the values for the "nonuniform" type of the value entry.

In our current development version, I have introduced a more flexible way of specifying the corresponding field entries. There, it can be not only "uniform" and "nonuniform" but also "linearProfile", "radialProfile", "fittedProfile" and so on.
But this not yet ready for release and also not yet documented.
( But in case you are interested: The same code is also used in the "extendedFixedValueBC" here: http://sourceforge.net/p/insightcae/...ions/openfoam/ )

For now you need a workaround. Some possibilities come into my mind:

1.)
If you don't mind a some programming, you could derive your own BC from the inflowGenerator-BC and set the fields in the "updateCoefficients" function. This also the only way if you need unsteadiness.

2.)
You create a dummy-copy of the field and specify some other BC, e.g. "groovyBC" or "timeVaryingMappedFixedValue", then you run the solver and let it compute and write a new timestep with the proper "nonuniform" value-statement in it. You can then copy this into your original field file and start the simulation with it.
I agree that this is pretty cumbersome. For that reason I started the new implementation...

Regards, Hannes
wyldckat, gentela, syavash and 2 others like this.
hannes is offline   Reply With Quote

Old   July 1, 2015, 03:10
Default
  #58
Senior Member
 
Syavash Asgari
Join Date: Apr 2010
Posts: 473
Rep Power: 18
syavash is on a distinguished road
Dear Foamers,

Unfortunately despite following the steps in Readme file, I encounter errors when trying to install LeMOS. The error message is as follows:

Code:
syavash@syavash-VPCF11DGX:~/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x$ ./Allwmake + wmake libso libLEMOS-2.3.x
/usr/bin/ld: cannot find -lgsl
collect2: error: ld returned 1 exit status
make: *** [/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/lib/libLEMOS-2.3.x.so] Error 1
+ cd applications
+ wmake all solvers
make[1]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/solvers/basic'
make[2]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/solvers/basic/PODSolver'
g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/libLEMOS-2.3.x/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/finiteVolume/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/meshTools/lnInclude  -IlnInclude -I. -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OpenFOAM/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OSspecific/POSIX/lnInclude   -fPIC -Xlinker --add-needed -Xlinker --no-as-needed Make/linux64GccDPOpt/PODSolver.o -L/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/lib \
         -lfiniteVolume -lmeshTools -lLEMOS-2.3.x -lOpenFOAM -ldl   -lm -o /home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/PODSolver
/usr/bin/ld: cannot find -lLEMOS-2.3.x
collect2: error: ld returned 1 exit status
make[2]: *** [/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/PODSolver] Error 1
make[2]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/solvers/basic/PODSolver'
make[1]: *** [PODSolver] Error 2
make[1]: Target `application' not remade because of errors.
make[1]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/solvers/basic'
make: *** [basic] Error 2
make[1]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/solvers/scalarPimpleFoam'
make[1]: `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/scalarPimpleFoam' is up to date.
make[1]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/solvers/scalarPimpleFoam'
make[1]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/solvers/scalarPimpleFoamLDMMS'
SOURCE=scalarPimpleFoamLDMMS.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/turbulenceModels/incompressible/turbulenceModel -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/transportModels -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/transportModels/incompressible/singlePhaseTransportModel -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/turbulenceModels/LES/LESfilters/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/finiteVolume/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/meshTools/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/fvOptions/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/sampling/lnInclude -IlnInclude -I. -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OpenFOAM/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/scalarPimpleFoamLDMMS.o
In file included from scalarPimpleFoamLDMMS.C:54:0:
createFields.H: In function ‘int main(int, char**)’:
createFields.H:106:13: error: ‘class Foam::incompressible::turbulenceModel’ has no member named ‘registerScalarField’
 turbulence->registerScalarField(f,D_f);
             ^
scalarPimpleFoamLDMMS.C:113:44: error: ‘class Foam::incompressible::turbulenceModel’ has no member named ‘molecularDiffusivityCoeff’
         volScalarField DEff =  turbulence->molecularDiffusivityCoeff(f.name()) + turbulence->turbulentDiffusivityCoeff(f.name());
                                            ^
scalarPimpleFoamLDMMS.C:113:94: error: ‘class Foam::incompressible::turbulenceModel’ has no member named ‘turbulentDiffusivityCoeff’
         volScalarField DEff =  turbulence->molecularDiffusivityCoeff(f.name()) + turbulence->turbulentDiffusivityCoeff(f.name());
                                                                                              ^
scalarPimpleFoamLDMMS.C:118:29: error: ‘class Foam::incompressible::turbulenceModel’ has no member named ‘divFeff’
               + turbulence->divFeff(f)
                             ^
make[1]: *** [Make/linux64GccDPOpt/scalarPimpleFoamLDMMS.o] Error 1
make[1]: Target `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/scalarPimpleFoamLDMMS' not remade because of errors.
make[1]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/solvers/scalarPimpleFoamLDMMS'
make: *** [scalarPimpleFoamLDMMS] Error 2
make[1]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/solvers/scalarPimpleFoamMFM'
SOURCE=scalarPimpleFoamMFM.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/turbulenceModels/incompressible/turbulenceModel -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/transportModels -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/transportModels/incompressible/singlePhaseTransportModel -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/turbulenceModels/LES/LESfilters/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/finiteVolume/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/meshTools/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/fvOptions/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/sampling/lnInclude -IlnInclude -I. -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OpenFOAM/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/scalarPimpleFoamMFM.o
In file included from scalarPimpleFoamMFM.C:54:0:
createFields.H: In function ‘int main(int, char**)’:
createFields.H:106:13: error: ‘class Foam::incompressible::turbulenceModel’ has no member named ‘registerScalarField’
 turbulence->registerScalarField(f,D_f);
             ^
scalarPimpleFoamMFM.C:113:44: error: ‘class Foam::incompressible::turbulenceModel’ has no member named ‘molecularDiffusivityCoeff’
         volScalarField DEff =  turbulence->molecularDiffusivityCoeff(f.name()) + turbulence->turbulentDiffusivityCoeff(f.name());
                                            ^
scalarPimpleFoamMFM.C:113:94: error: ‘class Foam::incompressible::turbulenceModel’ has no member named ‘turbulentDiffusivityCoeff’
         volScalarField DEff =  turbulence->molecularDiffusivityCoeff(f.name()) + turbulence->turbulentDiffusivityCoeff(f.name());
                                                                                              ^
scalarPimpleFoamMFM.C:118:29: error: ‘class Foam::incompressible::turbulenceModel’ has no member named ‘divFeff’
               + turbulence->divFeff(f)
                             ^
make[1]: *** [Make/linux64GccDPOpt/scalarPimpleFoamMFM.o] Error 1
make[1]: Target `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/scalarPimpleFoamMFM' not remade because of errors.
make[1]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/solvers/scalarPimpleFoamMFM'
make: *** [scalarPimpleFoamMFM] Error 2
make: Target `application' not remade because of errors.
+ cd applications
+ wmake all utilities
make[1]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing'
make[2]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/POD'
make[3]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/POD/scalarSnapshots'
g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/libLEMOS-2.3.x/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/finiteVolume/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/meshTools/lnInclude -IlnInclude -I. -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OpenFOAM/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OSspecific/POSIX/lnInclude   -fPIC -Xlinker --add-needed -Xlinker --no-as-needed Make/linux64GccDPOpt/scalarSnapshots.o -L/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/lib \
         -lfiniteVolume -lmeshTools -lLEMOS-2.3.x -lODE -lOpenFOAM -ldl   -lm -o /home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/scalarSnapshots
/usr/bin/ld: cannot find -lLEMOS-2.3.x
collect2: error: ld returned 1 exit status
make[3]: *** [/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/scalarSnapshots] Error 1
make[3]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/POD/scalarSnapshots'
make[2]: *** [scalarSnapshots] Error 2
make[3]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/POD/vectorSnapshots'
g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/libLEMOS-2.3.x/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/finiteVolume/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/meshTools/lnInclude -IlnInclude -I. -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OpenFOAM/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OSspecific/POSIX/lnInclude   -fPIC -Xlinker --add-needed -Xlinker --no-as-needed Make/linux64GccDPOpt/vectorSnapshots.o -L/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/lib \
         -lfiniteVolume -lmeshTools -lLEMOS-2.3.x -lODE -lOpenFOAM -ldl   -lm -o /home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/vectorSnapshots
/usr/bin/ld: cannot find -lLEMOS-2.3.x
collect2: error: ld returned 1 exit status
make[3]: *** [/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/vectorSnapshots] Error 1
make[3]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/POD/vectorSnapshots'
make[2]: *** [vectorSnapshots] Error 2
make[2]: Target `application' not remade because of errors.
make[2]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/POD'
make[1]: *** [POD] Error 2
make[2]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/miscellaneous'
make[3]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/miscellaneous/postChannelExt'
make[3]: `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/postChannelExt' is up to date.
make[3]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/miscellaneous/postChannelExt'
make[2]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/miscellaneous'
make[2]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/velocityField'
make[3]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/velocityField/LambdaCI'
make[3]: `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/LambdaCI' is up to date.
make[3]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/velocityField/LambdaCI'
make[2]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/velocityField'
make[1]: Target `application' not remade because of errors.
make[1]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing'
make: *** [postProcessing] Error 2
make: Target `application' not remade because of errors.
I am a newbie in OF and don't really understand where the problem lies. Could anyone help me with this issue?!
Thanks
syavash is offline   Reply With Quote

Old   July 1, 2015, 03:18
Default
  #59
Senior Member
 
Hannes Kröger
Join Date: Mar 2009
Location: Rostock, Germany
Posts: 123
Rep Power: 18
hannes is on a distinguished road
I see two problems:

1. Gnu Scientific Library (gsl) is not installed. Please install the "-dev" package of your distribution.

Quote:
Originally Posted by syavash View Post
Code:
/usr/bin/ld: cannot find -lgsl
2. You need to apply a patch to the OpenFOAM source to be able to compile the turbulence models. This patch adds some helper functions to the LESModel base class which were required for implementation of the DMM model.
There is a script "applyPatches" for that. Note that this requires write access to the OpenFOAM sources, i.e. you need to have OpenFOAM installed in your $HOME directory.

Quote:
Originally Posted by syavash View Post
Code:
createFields.H: In function ‘int main(int, char**)’:
createFields.H:106:13: error: ‘class Foam::incompressible::turbulenceModel’ has no member named ‘registerScalarField’
 turbulence->registerScalarField(f,D_f);
             ^
Hope that helps.

Regards, Hannes
gentela and Bazinga like this.
hannes is offline   Reply With Quote

Old   July 1, 2015, 04:14
Default
  #60
Senior Member
 
Syavash Asgari
Join Date: Apr 2010
Posts: 473
Rep Power: 18
syavash is on a distinguished road
Quote:
Originally Posted by hannes View Post
I see two problems:

1. Gnu Scientific Library (gsl) is not installed. Please install the "-dev" package of your distribution.



2. You need to apply a patch to the OpenFOAM source to be able to compile the turbulence models. This patch adds some helper functions to the LESModel base class which were required for implementation of the DMM model.
There is a script "applyPatches" for that. Note that this requires write access to the OpenFOAM sources, i.e. you need to have OpenFOAM installed in your $HOME directory.





Hope that helps.

Regards, Hannes

Dear Hannes,

Thanks for quick reply!
1-I have installed OF in my $Home directory and "applyPatches" script seems to execute properly.
2- As you suggested, I installed GNU Scientific Library (gsl 1.16) but now another error message appears after running Allwmake:

Code:
+ cd applications
+ wmake all solvers
make[1]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/solvers/basic'
make[2]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/solvers/basic/PODSolver'
g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/libLEMOS-2.3.x/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/finiteVolume/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/meshTools/lnInclude  -IlnInclude -I. -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OpenFOAM/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OSspecific/POSIX/lnInclude   -fPIC -Xlinker --add-needed -Xlinker --no-as-needed Make/linux64GccDPOpt/PODSolver.o -L/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/lib \
         -lfiniteVolume -lmeshTools -lLEMOS-2.3.x -lOpenFOAM -ldl   -lm -o /home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/PODSolver
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zher2k'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_dtrsm'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_ctrmm'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_csyrk'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_dsyr2k'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_dsyr'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_sgemm'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_srot'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_dzasum'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_idamax'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_csyr2k'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zhemv'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_drotm'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_dsymm'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zsyrk'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_sdsdot'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zgerc'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_ssyr2'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_cher'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zsymm'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_ztrsm'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_cher2k'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_sasum'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_ztrsv'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_ccopy'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_ztrmm'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_dger'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_dtrmv'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_izamax'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zdscal'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_sdot'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zdotu_sub'
collect2: error: ld returned 1 exit status
make[2]: *** [/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/PODSolver] Error 1
make[2]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/solvers/basic/PODSolver'
make[1]: *** [PODSolver] Error 2
make[1]: Target `application' not remade because of errors.
make[1]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/solvers/basic'
make: *** [basic] Error 2
make[1]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/solvers/scalarPimpleFoam'
make[1]: `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/scalarPimpleFoam' is up to date.
make[1]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/solvers/scalarPimpleFoam'
make[1]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/solvers/scalarPimpleFoamLDMMS'
SOURCE=scalarPimpleFoamLDMMS.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/turbulenceModels/incompressible/turbulenceModel -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/transportModels -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/transportModels/incompressible/singlePhaseTransportModel -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/turbulenceModels/LES/LESfilters/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/finiteVolume/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/meshTools/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/fvOptions/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/sampling/lnInclude -IlnInclude -I. -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OpenFOAM/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/scalarPimpleFoamLDMMS.o
In file included from scalarPimpleFoamLDMMS.C:54:0:
createFields.H: In function ‘int main(int, char**)’:
createFields.H:106:13: error: ‘class Foam::incompressible::turbulenceModel’ has no member named ‘registerScalarField’
 turbulence->registerScalarField(f,D_f);
             ^
scalarPimpleFoamLDMMS.C:113:44: error: ‘class Foam::incompressible::turbulenceModel’ has no member named ‘molecularDiffusivityCoeff’
         volScalarField DEff =  turbulence->molecularDiffusivityCoeff(f.name()) + turbulence->turbulentDiffusivityCoeff(f.name());
                                            ^
scalarPimpleFoamLDMMS.C:113:94: error: ‘class Foam::incompressible::turbulenceModel’ has no member named ‘turbulentDiffusivityCoeff’
         volScalarField DEff =  turbulence->molecularDiffusivityCoeff(f.name()) + turbulence->turbulentDiffusivityCoeff(f.name());
                                                                                              ^
scalarPimpleFoamLDMMS.C:118:29: error: ‘class Foam::incompressible::turbulenceModel’ has no member named ‘divFeff’
               + turbulence->divFeff(f)
                             ^
make[1]: *** [Make/linux64GccDPOpt/scalarPimpleFoamLDMMS.o] Error 1
make[1]: Target `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/scalarPimpleFoamLDMMS' not remade because of errors.
make[1]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/solvers/scalarPimpleFoamLDMMS'
make: *** [scalarPimpleFoamLDMMS] Error 2
make[1]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/solvers/scalarPimpleFoamMFM'
SOURCE=scalarPimpleFoamMFM.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/turbulenceModels/incompressible/turbulenceModel -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/transportModels -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/transportModels/incompressible/singlePhaseTransportModel -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/turbulenceModels/LES/LESfilters/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/finiteVolume/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/meshTools/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/fvOptions/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/sampling/lnInclude -IlnInclude -I. -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OpenFOAM/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/scalarPimpleFoamMFM.o
In file included from scalarPimpleFoamMFM.C:54:0:
createFields.H: In function ‘int main(int, char**)’:
createFields.H:106:13: error: ‘class Foam::incompressible::turbulenceModel’ has no member named ‘registerScalarField’
 turbulence->registerScalarField(f,D_f);
             ^
scalarPimpleFoamMFM.C:113:44: error: ‘class Foam::incompressible::turbulenceModel’ has no member named ‘molecularDiffusivityCoeff’
         volScalarField DEff =  turbulence->molecularDiffusivityCoeff(f.name()) + turbulence->turbulentDiffusivityCoeff(f.name());
                                            ^
scalarPimpleFoamMFM.C:113:94: error: ‘class Foam::incompressible::turbulenceModel’ has no member named ‘turbulentDiffusivityCoeff’
         volScalarField DEff =  turbulence->molecularDiffusivityCoeff(f.name()) + turbulence->turbulentDiffusivityCoeff(f.name());
                                                                                              ^
scalarPimpleFoamMFM.C:118:29: error: ‘class Foam::incompressible::turbulenceModel’ has no member named ‘divFeff’
               + turbulence->divFeff(f)
                             ^
make[1]: *** [Make/linux64GccDPOpt/scalarPimpleFoamMFM.o] Error 1
make[1]: Target `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/scalarPimpleFoamMFM' not remade because of errors.
make[1]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/solvers/scalarPimpleFoamMFM'
make: *** [scalarPimpleFoamMFM] Error 2
make: Target `application' not remade because of errors.
+ cd applications
+ wmake all utilities
make[1]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing'
make[2]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/POD'
make[3]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/POD/scalarSnapshots'
g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/libLEMOS-2.3.x/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/finiteVolume/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/meshTools/lnInclude -IlnInclude -I. -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OpenFOAM/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OSspecific/POSIX/lnInclude   -fPIC -Xlinker --add-needed -Xlinker --no-as-needed Make/linux64GccDPOpt/scalarSnapshots.o -L/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/lib \
         -lfiniteVolume -lmeshTools -lLEMOS-2.3.x -lODE -lOpenFOAM -ldl   -lm -o /home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/scalarSnapshots
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zher2k'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_dtrsm'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zhemm'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_sdot'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zdotu_sub'
collect2: error: ld returned 1 exit status
make[3]: *** [/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/scalarSnapshots] Error 1
make[3]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/POD/scalarSnapshots'
make[2]: *** [scalarSnapshots] Error 2
make[3]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/POD/vectorSnapshots'
g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/libLEMOS-2.3.x/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/finiteVolume/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/meshTools/lnInclude -IlnInclude -I. -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OpenFOAM/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OSspecific/POSIX/lnInclude   -fPIC -Xlinker --add-needed -Xlinker --no-as-needed Make/linux64GccDPOpt/vectorSnapshots.o -L/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/lib \
         -lfiniteVolume -lmeshTools -lLEMOS-2.3.x -lODE -lOpenFOAM -ldl   -lm -o /home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/vectorSnapshots
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zher2k''
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zdotc_sub'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_strmm'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_csymm'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_sger'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zscal'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_srotg'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_strmv'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_cgerc'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_saxpy'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_cherk'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_dsdot'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_ssymv'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zher2'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_ddot'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_dnrm2'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_cgemv'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zgemv'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_ctrmv'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_cswap'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zgemm'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_ctrmm'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_csyrk'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_dsyr2k'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_dsyr'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_sgemm'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_srot'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_dzasum'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_idamax'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_csyr2k'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zhemv'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_drotm'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_dsymm'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zsyrk'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_sdsdot'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zgerc'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_ssyr2'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_cher'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zsymm'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_ztrsm'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_cher2k'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_sdot'
//usr/local/lib/libgsl.so.0: undefined reference to `cblas_zdotu_sub'
collect2: error: ld returned 1 exit status
make[3]: *** [/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/vectorSnapshots] Error 1
make[3]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/POD/vectorSnapshots'
make[2]: *** [vectorSnapshots] Error 2
make[2]: Target `application' not remade because of errors.
make[2]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/POD'
make[1]: *** [POD] Error 2
make[2]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/miscellaneous'
make[3]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/miscellaneous/postChannelExt'
make[3]: `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/postChannelExt' is up to date.
make[3]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/miscellaneous/postChannelExt'
make[2]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/miscellaneous'
make[2]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/velocityField'
make[3]: Entering directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/velocityField/LambdaCI'
make[3]: `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/LambdaCI' is up to date.
make[3]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/velocityField/LambdaCI'
make[2]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing/velocityField'
make[1]: Target `application' not remade because of errors.
make[1]: Leaving directory `/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/LEMOS-2.3.x/applications/utilities/postProcessing'
make: *** [postProcessing] Error 2
make: Target `application' not remade because of errors.
Do you have any idea how to resolve that??!

Regards
Syavash
Last edited by syavash; July 1, 2015 at 05:30.
syavash is offline   Reply With Quote

Reply
Page 3 of 6 12 3 45 Last »

Tags
inflow conditions, lemos

« Previous Thread | Next Thread »

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


All times are GMT -4. The time now is 20:17.

Contact Us - CFD Online - Privacy Statement - Top