Usage of runTimePostProcessing
2 Attachment(s)
Hi folks,
I would like to make a movie from a DNS-Simulation. Therefore I want to safe fotos(frames) from each time step. My Domain is a simple cube with turbulence inside. I work with OF-1712 sine this special DNS-Solver only exists for this version. The only fuction I know to produce scuch "screenshots" is: runTimePostProcessing Unfortunatelly there is noproper guide for it. The examples in the tutorials and other websites helped only a little. Let's say, I want to make a picture of this cube-domain visualising velocity. You find attached the settings of the runTimePostProcessing as well as the log file with the sim-feedback. Sooo, what I've done wrong? What would be the right syntax here? Maybe somebody has a good example file? Thank you in advance. Attachment 80354 Attachment 80355 |
maybe helpful. I use paraview to make movie. run it parallelly.
save as movies directly or step time picture, both are OK. |
Thanks bestucan, but I really do not want to safe the results before reading them in paraview. I want to make the movie from the calculation without saving the profiles. Otherwise it would need many terrabytes and a lot of cpu-power would be lost for the saving
|
Solution ?
Quote:
Any updates how one can output pictures as jpeg/png and write out every time step or duration? Please post the solution if you have found :D |
Quote:
That is what was used to make the laser melting video. Was a bit of overkill writing png images each time step since it would have made the video far too lengthy, but nonetheless cool. Using runTimePostPro should generally be the fastest, since you can reuse OpenFOAM sampled elements etc and don't have pass things through paraview at all. However, probably only useful for production runs since setting up scenes is a bit of a pain. The Catalyst viz is certainly a bit more wysiwyg Take a look at the video: https://vimeo.com/277640232 |
Quote:
The problem is we are running transient analysis on cluster, on cluster the png creation is fast using runTimePostPro. Also additional software installation like Catalyst need extra costs. The runTimePostPro tutorial is the best option on cluster. But I am not how to implement it from the tutorials using ("librunTimePostProcessing.so"); libraries. |
Quote:
The wind around buildings is perhaps the most extensive example. In general, you would want to take some portion of an existing simulation and then use that for doing the setup (eg, solverName -postProcess) for runTimePostProcessing. There is unfortunately not as much documentation as would be nice (will likely need to explore the source code as well). If you do get something interesting that could either be added to an existing tutorial, or add a new one, this would be a most welcome contribution. That way others can benefit too. Once it gets that far, please open an issue on develop.openfoam.com to get your tutorial added OR perhaps through the tutorials wiki (https://wiki.openfoam.com/index.php?title=Tutorials) |
Quote:
Code:
|
Did you compile VTK with osmesa?
|
Quote:
How do I check if it is compiled with osmesa? Update: Never mind, I had to check if any libvtk*.so has a dependency on osmesa using ldd command. I think the VTK version used during the OpenFOAM building was not built with osmesa. |
I got runTimePostProcessing function object running.
0) Install osmesa, on Ubuntu 22.04: Code:
sudo apt install libosmesa6 libosmesa6-dev 2) cd to VTK directory and create a directory 'build' and cd to it. 3) run: Code:
ccmake .. -DVTK_OPENGL_HAS_OSMESA=ON 4) Now, to find the VTK module required by the runTimePostProcesisng function object, clone the openfoam repository and the visualization module. 5) cd to the runTimePostProcessing directory and find the required modules by running: Code:
grep -r 'VTK::' 7) Compile vtk and install it Code:
Code:
9) Clone OpenFOAM repository (skip if you did in step 4). 10) Build OpenFOAM. 11) Compile the runTimePostProcessing library. 12) If you have tried step (8*) make sure to remove the librunTimePostProcessing.so from $FOAM_USER_LIBBIN and $FOAM_LIBBBIN and replace them with the newly compiled one after building OpenFOAM from source. 13) You must run this to get it to work for this session to load (you need to run this only this time): Code:
sudo ldconfig The steps above are not perfect but they should work. |
All times are GMT -4. The time now is 15:22. |