I am not quite sure what this error is referring to. Is it a numerical issue, or is the physical system I have set up unrealistic? (It may be worth noting that I have successfully run Eulerian-Eulerian simulations with twoPhaseEulerFoam that match experimental data quite well). I have attached my inputs as a tar.zip, as well as a text file with the stdout from the simulation.
My simulations are comprised of a ~8 m quarter cylinder pipe with ~0.1 m diameter. A fully developed, single phase (comprised of water) turbulent flow is injected at the inlet. 0.01 m downstream of the inlet, there is a small band on the wall at which gas is injected with wall-normal velocity. The gas-water mixture then traverses 8 m of pipe until it reaches the outlet, at which a zero gradient BC is applied.
I am completely unsure how to go about addressing this issue, any help would be much appreciated!
Post by Alberto Passalacqua on Nov 18, 2019 2:17:21 GMT -6
before I start looking at your case, could you tell me what version of OpenQBMM you are using?
Specifically, if you are using OpenQBMM 5 for OpenFOAM 7, there was an issue in the generateMoment utility, which is now corrected in OpeQBMM 5.0.1 (and in the master branch). If you used git to download the code, you can update as follows:
Thank you for getting back to me! I've attached the polyMesh directory as a tar.xz. It was generated using the meshing software Cubit v14 and then converting the .msh file to an OpenFOAM mesh using the fluent3DMeshToFoam utility. The output from these steps are given in the cubit.log and fluent3DMeshToFoam.log text files, respectively, in the attachment on my first post.
I am actually using OpenQBMM 4 with OpenFOAM 6. I have been working with OpenFOAM 6 for some time, and recall reading that OpenQBMM 4 was the last version designed to work with this version of OpenFOAM. Are there any issues with this combination that I should be aware of?
I could also upgrade both OpenFOAM and OpenQBMM, if you think that would resolve this issue.
Post by Alberto Passalacqua on Nov 22, 2019 18:12:12 GMT -6
Thank you for sharing the mesh. I will take a look.
The changes that led to the issue I mentioned happened after OpenQBMM 4 was released. However, the polydisperseBubbleFoam solver was modified to make it more robust. Likely, the error you are seeing is due to the the "flux corrector". You can set the nFluxCorrector to 0 in the fvSolution/PIMPLE subdictionary, and it will likely resolve the problem. The price you pay is a small inconsistency in the solution between the zero-order moment and the advected volume fraction. This algorithm has improved in OpenQBMM 5.0: we worked to make it more robust. However, in some cases, the flux corrector is still giving some issue (and the correction is usually small anyway, so it is safe to disable it: just check the alpha - m0 consistency). A complete solution implies re-designing the numerical scheme for mean transport. It's on my radar, but it will take some time.
Post by Alberto Passalacqua on Nov 23, 2019 21:03:52 GMT -6
I have ported the case to OpenQBMM 5.0.1 (See attachment). I assume water is the continuous phase (check populationBalanceProperties dictionary, kernel settings). I also took the liberty of making a modification to the GAMG settings: nCellsInCoarsestLevel should be ~sqrt(nCells)).
I have only ran it for a short time on 4 CPUs and it seems to be fine. If you run it to completion, please let me know if the issue is addressed.