|
[Sponsors] |
June 9, 2010, 09:42 |
problem with chtMultiRegionFoam tutorial...
|
#1 |
Senior Member
Cyprien
Join Date: Feb 2010
Location: Stanford University
Posts: 299
Rep Power: 18 |
Hi everybody !
I was trying to run the chtMultiRegionFoam/multiRegionHeater by the ./Allrun command. Some log files are creating, but it look as if nothing happens : the only directory remains the "0" folder. I try another way (according to an online presentation) executing the following commands: blockMesh -> OK setSet -batch makeCellSets.setSet -> here I get the following error message Code:
setSet: error while loading shared libraries: libreadline.so.5: cannot open shared object file: No such file or directory Thank you for your help, Cyp |
|
June 9, 2010, 10:35 |
|
#2 | |
Member
Join Date: Jun 2010
Posts: 31
Rep Power: 15 |
Try this in Terminal:
Quote:
|
||
June 9, 2010, 10:37 |
|
#3 |
Senior Member
Cyprien
Join Date: Feb 2010
Location: Stanford University
Posts: 299
Rep Power: 18 |
thank you for your answer
in which directory do I apply your command line ?? |
|
June 9, 2010, 10:45 |
|
#4 |
Member
Join Date: Jun 2010
Posts: 31
Rep Power: 15 |
||
June 9, 2010, 10:58 |
|
#5 |
Senior Member
Cyprien
Join Date: Feb 2010
Location: Stanford University
Posts: 299
Rep Power: 18 |
I still have the same problem...
|
|
June 10, 2010, 09:39 |
|
#6 |
Member
Robertas N.
Join Date: Mar 2009
Location: Kaunas, Lithuania
Posts: 53
Rep Power: 17 |
Try this:
ldd `which setSet` and see if it can find libreadline.so.5. Is this file really present somewhere in /lib or /usr/lib? BTW, I ran this on my PC and it seems that setSet does not even depend on libreadline... It would be helpful if you could inform that distro/version and OF version you are using (that's the first thing to do when asking questions like this). |
|
June 10, 2010, 12:04 |
|
#7 |
Senior Member
Cyprien
Join Date: Feb 2010
Location: Stanford University
Posts: 299
Rep Power: 18 |
Hi !
when I type your command, I get : Code:
libreadline.so.5 => not found Code:
kde4-config: /USER/OpenFOAM/ThirdParty-1.6/gcc-4.3.3/platforms/linux64/lib64/libstdc++.so.6: version `GLIBCXX_3.4.11' not found (required by /usr/lib64/libkdecore.so.5) kde4-config: USER/OpenFOAM/ThirdParty-1.6/gcc-4.3.3/platforms/linux64/lib64/libstdc++.so.6: version `GLIBCXX_3.4.11' not found (required by /usr/lib64/libkdecore.so.5) I have a OpenSuSe 11.2 and I run OpenFOAM 1.6 |
|
June 10, 2010, 12:13 |
|
#8 |
Senior Member
Cyprien
Join Date: Feb 2010
Location: Stanford University
Posts: 299
Rep Power: 18 |
I saw a similar topic :
http://www.cfd-online.com/Forums/ope...-tutorial.html but there is no tips that can help me |
|
June 10, 2010, 12:46 |
|
#9 | ||
Member
Robertas N.
Join Date: Mar 2009
Location: Kaunas, Lithuania
Posts: 53
Rep Power: 17 |
Quote:
about this lib under O-suse. Quote:
is "substituted" by the OF library, because of the OF/etc/bashrc script. Try to open the console, do not source the OF/etc/bashrc, and then run an editor. See if it works. Make sure sourcing OF/etc/bashr is not included in your (or system-wide) .bashrc script. Also you may try some text-mode editor, like 'vim' or similar. These are just some quick guesses, I'm not sure if this helps, but maybe you'll notice smth informative. |
|||
June 11, 2010, 11:36 |
|
#10 |
Senior Member
Cyprien
Join Date: Feb 2010
Location: Stanford University
Posts: 299
Rep Power: 18 |
thank you r08n your very good advices. I have installed the libreadline5 librairie, and now my calculation successfully ran.
I encounter a new problem now : I can't view any fields with paraFoam. Do you have any idea ? |
|
June 14, 2010, 10:35 |
|
#11 | |
Member
Robertas N.
Join Date: Mar 2009
Location: Kaunas, Lithuania
Posts: 53
Rep Power: 17 |
Quote:
1) after setting up the geometry with multiple regions (with setSet, setsToZones, splitMeshRegions), a new folder is created 0.001. It contains a separate folder for each region, and each such subfolder contains a folder "polyMesh"; e.g., case_name/0.001/region1/polyMesh/, etc. 2) while running the simulation, appropriate folders for times are created, as usual. 3) Now, after the simulation ends, link or copy the folder "polyMesh" from time 0.001 subfolder of appropriate region into the subfolders of respective regions in other time folders; e.g. 0.001/region1/polyMesh --> 10.001/region1/polyMesh, 0.001/region2/polyMesh --> 10.001/region2/polyMesh, etc. Repeat for all the regions and times like this: for t in 10.001 20.001 30.001 ... do for r in region1 region2 ... do ln -s 0.001/$r/polyMesh $t/$r/polyMesh done done 4) from within the case folder, run foamToVTK for each region: foamToVTK -useTimeName -region region1 etc. (repeat for each region). This should create a folder with the structure like this: case_name/VTK/region1/grid_10.001.vtk etc., i.e., .vtk files for each region and time. 5) run 'paraview' (not paraFoam) and open these *.vtk files. There are instructions here: http://openfoamwiki.net/index.php/Ho...rocMultiregion but it seems that I used a slightly different procedure, as described above. I'm not sure if I was doing the things right. Any comments? |
||
June 14, 2010, 10:39 |
|
#12 |
Senior Member
Cyprien
Join Date: Feb 2010
Location: Stanford University
Posts: 299
Rep Power: 18 |
thank you very much for your answer !
Indeed, it perfectly works when I use paraview instead of paraFoam |
|
June 14, 2010, 10:58 |
|
#13 |
Member
Join Date: Jun 2010
Posts: 31
Rep Power: 15 |
Hello ro8n,
The following is my procedure for viewing fields in multiple regions in the multiRegionHeater tutorial: 5. Create the remaining constant folders by entering the following commands in Terminal: mkdir constant/heater mkdir constant/leftSolid mkdir constant/rightSolid 6. Softlink the mesh from the first time step of each region to the constant directory of each region by entering the following commands in Terminal: cd constant/bottomAir ln -s ../../0.001/bottomAir/polyMesh polyMesh cd ../../ cd constant/topAir ln -s ../../0.001/topAir/polyMesh polyMesh cd ../../ cd constant/heater ln -s ../../0.001/heater/polyMesh polyMesh cd ../../ cd constant/leftSolid ln -s ../../0.001/leftSolid/polyMesh polyMesh cd ../../ cd constant/rightSolid ln -s ../../0.001/rightSolid/polyMesh polyMesh cd ../../ 7. Convert the format of each region to VTK by entering the following commands in Terminal: foamToVTK -region bottomAir foamToVTK -region topAir foamToVTK -region heater foamToVTK -region leftSolid foamToVTK -region rightSolid 8. Run ParaView by entering the following command in Terminal: paraFoam 9. Open the following folders in ParaView: VTK/bottomAir/multiRegionHeater_..vtk VTK/topAir/multiRegionHeater_..vtk VTK/heater/multiRegionHeater_..vtk VTK/leftSolid/multiRegionHeater_..vtk VTK/rightSolid/multiRegionHeater_..vtk best regards, Matt |
|
June 15, 2010, 06:17 |
|
#14 | |
Member
MSarkar
Join Date: Dec 2009
Posts: 99
Rep Power: 16 |
Quote:
I faced same problem to visualize the results from multi-region simulation and followed your instructions to convert the results to VTK format but it did not work for me. It created all region folders within VTK folder and region folder it creates caseName_time.vtk file (caseName/VTK/region/caseName_time.vtk) but I am not able to visualize the field values (like p, T, U etc). Only I can see the mesh. When I uploaded this vtk file in paraview it gives me option to display Solid Color, CellID and cellNormals, no field name like p, U, T etc. I followed your suggestion exactly but I don't know what is wrong there. Please help me to visualize the results. I ran chtMultiRegionFoam solver and I am using OF-1.6.x version (freefoam). Thanks M. Sarkar |
||
June 18, 2010, 06:05 |
|
#15 | ||
Member
Robertas N.
Join Date: Mar 2009
Location: Kaunas, Lithuania
Posts: 53
Rep Power: 17 |
Quote:
and see if there any field data; for example, for the field 'rho' there must be a string like 'rho 1 130 float' and then some numbers in binary (looks like random symbols) or ascii format. Before running foamToVTK, is there field data (the files for U, T, rho, phi, etc. as appropriate) in the appropriate time and region subfolders (e.g., 20.001/region1/U , etc)? Are the polyMesh folders in region folders linked to respective region folders in 0.001? (e.g., 10.001/reg1/polyMesh --> 0.001/reg1/polyMesh; i.e., if there are no mixups between different regions). These are some quick guesses that came to mind. Quote:
|
|||
June 28, 2010, 03:48 |
|
#16 |
Member
MSarkar
Join Date: Dec 2009
Posts: 99
Rep Power: 16 |
Hello Robertas,
I think it was my bad, I did not open right vtk file. Now I am able to visualize the results. Thanks a lot for you post. Regards M. Sarkar |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Problem on Fluent Tutorial: Horizontal Film Boilig | Feng | FLUENT | 2 | April 13, 2013 05:34 |
newbie problem with cavity tutorial | miki | OpenFOAM Running, Solving & CFD | 8 | September 2, 2012 15:22 |
Problem setting with chtmultiregionFoam | Antonin | OpenFOAM | 10 | April 24, 2012 09:50 |
Help! Compiled UDF problem 4 Wave tank tutorial | Shane | FLUENT | 1 | September 3, 2010 02:32 |
Adiabatic and Rotating wall (Convection problem) | ParodDav | CFX | 5 | April 29, 2007 19:13 |