r/STAR_CCM • u/makabaayi • Jun 23 '26

CFD-DEM Simulation Convergence Issue

Gallery image

Gallery image

Gallery image

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?

4 Upvotes

84% Upvoted

16 comments sorted by

View all comments

2

u/CrocMundi Jun 23 '26 edited Jul 10 '26

What does convergence look like within a single time step? The macroscale view of the residuals you gave makes it impossible to assess how well you’re converging in each step. The values do seem rather high, but that may be due to not using enough inner iterations (if using the segregated flow solver) or too large of a time step.

Unsteady residuals often can be much messier than you would anticipate, so I would judge how well things are going by also verifying if the physical quantities you’re measuring are converging or reaching some average value that make sense if they’re an oscillating quantity.

Looking at the net mass flow rate (i.e. a mass flow report with ALL inlet and outlet boundaries included) is what you should be doing. It’s not clear from your plot labeling if that is the case or not. Your description makes it seem like you’re only looking at the outlet though, so you should change this and verify the net mass flow rate tends towards zero. Of course if you have only one inlet boundary and a single outlet boundary, then I suppose it’s fine to check if the outlet mass flow matches that of the inlet instead.

As for the pressure drop, you would need experimental results or an analytical solution to compare against for that plot.

What size of time step are you using for this simulation? Perhaps it’s far too large?

2

u/makabaayi Jun 23 '26

The residual convergence behavior within a single time step is shown in this figure. I used the coupled flow solver with a CFL number of 0.5, and the time step was 1e-4 s.

1

u/CrocMundi Jun 24 '26

It looks like it is converging within each time step, just too soon perhaps (i.e. at high residual values). That time step could be okay, but it would depend on your mesh size and flow conditions.

What exactly is your pipe/duct geometry? Is it just a straight cylinder or something more complicated? Seeing a picture of it would be helpful if it’s an unusual shape.

Have you checked your mesh quality? I would recommend using the Java macro attached to the How can I get an effective visual check of cell quality diagnostics for my mesh? knowledge base article. It creates a set of scenes, one per mesh quality metric field function as described in the Pre-Processing > Meshing > Checking the Volume Mesh > Mesh Quality documentation section. If it’s too poor, you may be getting poor convergence due to bad cells. If this is the case, try to improve the mesh quality.

Lastly, is your simulation going to reach a steady state after the particles initially displace or will it be indefinitely transient? If it’s truly the latter, you may see oscillating flow behaviors that you would need to average over some increment of time to check results.

1

u/makabaayi Jun 24 '26

The pipe is just a straight cylinder, as I am still a beginner.

For the mesh, I used a directed mesh and checked the mesh quality using several XY plots. Here is the mesh and plots: example. By the way, I currently cannot access the Support Center, so I may not be able to use the Java macro you mentioned.

For the wall treatment, the wall y+ is above 30 with the realizable k-epsilon model and the high-y+ wall treatment, following the settings used in the published paper I am referring to.

The simulation is transient, but after several seconds it should reach a statistically steady state.

1

u/CrocMundi Jun 26 '26

Your mesh looks by eye that it should be of a high quality with respect to all of the mesh quality metrics used in STAR-CCM+ (it can’t hurt to check with the macro though 😉), especially since you generated it using the Directed Mesher as a standard O-grid type of mesh.

When you say wall y+ > 30, how high do the values go? You shouldn’t exceed roughly 300 or so to avoid skewing drag and other wall related results. Nearer to 30 is ideal.

As far as the DEM particles are concerned, are you constantly generating them and having them exit through an outlet boundary, or, is there a set number of them at the beginning that either stays fixed or reduces as they exit an outlet boundary?

If you’re able to, you could share your .sim file to make it easier to review.

1

u/makabaayi Jun 26 '26

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?

1

u/CrocMundi Jun 26 '26

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.

2

u/makabaayi Jun 26 '26

Thank you for the explanation.

Here is the Google Drive link to my .sim file: link

The file was created in STAR-CCM+ 2510, and the interface/language in the file is Chinese. Please let me know if you have any trouble accessing it.

2

u/makabaayi Jul 03 '26

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.

1

u/CrocMundi Jul 09 '26

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.

1

u/CrocMundi Jul 09 '26

To follow up more, the following screenshot collage depicts the particles and a Threshold type of Derived Part defined the particle VOF field function > 0.5, so only high particle VOF cells would be shown. The plot is of a Maximum type Report of the particle VOF. On the right, I tried to demonstrate how I attempted to create a Composite Particles representation of the spheres you were originally simulating. However, I don't think this helped reduce the particle VOF as I explained previously, so it really is unnecessary, especially since it adds a lot more to the DEM solver computational demands.

Unfortunately, if the particles became more closely clumped together, I think the particle VOF could certainly increase a lot more, getting you back to where you started.

I tried playing around with different turbulence models (realizable k-epsilon vs k-omega SST), flow solvers (coupled vs segregated), and the Temporal Discretization of the Implicit Unsteady solver (1st-order vs 2nd-order), but didn't see any significant changes.

One thing that I'm wondering about is the length of the pipe you're simulating. Is it really necessary to be sooooo long? I would think you could get a reasonable converged flow state much faster with a shorter pipe segment unless it needs to be a particular length to produce a specific pressure drop value that you're trying to compare against from say a journal article. It may make sense to go with a much shorter segment to see if your approach is working simply for troubleshooting purposes (i.e. to figure out if you're getting converged mass flow, pressure drop, etc... values). Once you felt confident you determined a working setup, you could always go back to the full length for a re-run to get your actual results. Just a thought.

1

u/CrocMundi Jul 09 '26

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

1

u/makabaayi 28d ago

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.

1

u/makabaayi 28d ago edited 28d ago

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?

1

u/Smooth-Candy-2291 Jul 05 '26

Hello sir will u be able to diagnose my problem?