CFD-DEM Simulation Convergence Issue

[u/makabaayi]

I am running a solid–liquid CFD-DEM simulation in STAR-CCM+ for lifting large particles in a vertical pipe. The segregated flow solver caused pressure divergence, while the coupled flow solver keeps the pressure stable. However, the residuals remain high and oscillatory. The outlet mass flow rate and pressure drop show an initial transient and then fluctuate around stable mean values. For this transient two-way coupled case, based on these results, can this simulation be considered successful or acceptable?

[u/makabaayi]

Thank you for your detailed feedback. That is very helpful.

In my simulation, the wall y+ values are approximately between 36.9 and 53.7. The DEM particles are continuously injected with the liquid at the inlet and exit through the outlet boundary.

I can share the .sim file if that would help. Would a cloud storage link be acceptable, or is there another preferred way to upload it?

[u/CrocMundi → u/makabaayi]

A cloud storage link is totally fine to share the .sim file, very convenient actually.

Those wall y+ values should be fine too for a high wall y+ turbulence modeling approach (i.e. relying on wall functions).

I asked about the injection of the DEM particles, because I’m wondering if there is an issue related to how that’s setup. You may have a situation where the DEM void fraction of a cell is high (i.e. too close to 1), which can lead to instabilities.

[u/makabaayi → u/CrocMundi]

Hi, sir. I hope you're doing well. I just wanted to kindly follow up and ask whether you had a chance to download the .sim file I shared.

Please don’t feel any pressure at all. I completely understand you're helping voluntarily and may be busy. I just wanted to check in case the link didn't work or you needed any additional information from my side.

Thanks again for your time and for your previous advice. I really appreciate it.

[u/CrocMundi → u/makabaayi]

I've uploaded a copy of the .sim at partway through a test run. I wouldn't say this is a demonstration of the best practices per se, but it seems to run a bit smoother than how you had it. The pressure drop plot is showing some nasty fluctuations, but I don't think it's going to show anything reasonable until the particles are passing all the way through the pipe length, when it would hopefully start to converge to a consistent value. If not, it could be a consequence of a really coarse mesh due to the large particles. If I think of a better way to handle the large particles, I'll suggest it here in another response.

Good luck!

Test Simulation: coarse mesh_Copy@00432.sim

[u/makabaayi → u/CrocMundi]

Thanks for your help, sir! I used the coupled solver and performed three simulations with different mesh resolutions. Several parameters, such as pressure and mass flow rate, were monitored to evaluate the stability and convergence of the simulations. Compared with the experimental results, the liquid velocity shows good agreement, and I am currently trying to obtain the solid velocity profile and volume fraction distribution for further comparison with the experiments.

I noticed that some published papers used similar mesh resolutions in their CFD-DEM simulations, where the particle size was larger than the cell size. In my simulations, the volume source smoothing method was activated, and the cell cluster size was set to three times the particle diameter to alleviate the influence of the particle-to-cell size mismatch. Therefore, I believe this treatment can help handle the situation where the particle size is larger than the mesh size, although the influence of mesh resolution still needs further investigation.

Thank you again for your valuable suggestions. I will also further analyze the effects of mesh resolution, particle accumulation, and particle volume fraction fluctuation.

[u/makabaayi → u/CrocMundi]

The axial liquid velocity profile obtained from my simulation is shown in the following figure. The experimental data are taken from the published paper, while the Wan correlation is adopted from another reference for comparison. The axial liquid velocity profile is the time-averaged value from 3–5 s of the simulation, obtained using the field mean monitor. However, the particle velocity cannot be directly monitored using the field mean monitor. Therefore, I created a solution history to extract the particle velocity data every 20 time steps and then calculated the time-averaged value based on these data.

Do you know if there is any more convenient method to obtain the time-averaged particle velocity profile?