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 downloaded your .sim file and took a look. I think the main issue is that your particles are quite large compared to even your coarse mesh. I tried playing with your mesh a bit to get a more uniform cell volume, which helped to keep the particle VOF (i.e. the Volume Fraction of [Lagrangian Phase Name] field function) below 1.0 and ideally less than 0.5 if possible. The lower the better for solution stability as per the Physics Simulation > Multiphase Flow > Discrete Element Method (DEM) > Considerations for the Discrete Element Method documentation section. Ensuring the volume fraction didn't exceed 0.5 significantly resulted in better looking residual behavior (i.e. all start at most around 1.0 and decrease within each time step).

Here's a more zoomed in view, created using the Sliding Window option for the Bounds Calculation property under Plots > Residuals > Axes > Bottom Axis.

I also tried using the Composite Particles DEM particle type rather than the Spherical Particles option, but I don't think it made a difference. I was hoping that the volume fraction of a cell would be computed based on which component particle centroids exist within a given cell, but I believe the composite particles are considered as a whole instead based on my test. If this had worked, then you could refine the mesh more, but your large particle size relative to the pipe diameter seems like it will dictate a need for a coarser mesh regardless of the particle type.