Hello,
I need help from this forum to run this case and get some results by early next week. I am trying to simulate flow through a DPI that involves a vessel, tube and hemispherical cup as shown in the attached paper.
I built the model for the geometry shown in this paper from scratch and used a single body (single stl file) and applied all the boundary conditions. I ensured that there is no gap between the vessel and the cup. Everything is together. This model is for single-phase flow only. No particles involved. It has 2 million mesh point. I am trying to run. It starts running but then it blows up. I have checked all facts of the model, went through the 25.3 Users guide and is unable to determine why this is happening.
I sincerely request you to review this model and please help me in running this case.
The zipped file is large and I have uploaded this to google drive and shared the link. Anybody with this link can access the files. Everything is in the Zipped file.
I look forward to some help in this regard from this forum and hearing from you.
Once this single phase model runs, I need to develop a model with particles.
Thanks and Best Regards,
Sincerely,
Debashis
starts running
alfano-et-al-2021-full-scale-dem-simulation-of-coupled-fluid-and-dry-coated-particle-flow-in-swirl-based-dry-powder.pdf (6.9 MB)
I am getting this. Simulation time staying at 0. Don’t know why ? I also went over this website 13. Frequently asked questions — MFiX 25.3 documentation and unable to find any explanation for that.
Have you inspected your mesh and adjusted some meshing tolerances?
Dr. Dietiker,
Thank you very much for your reply.
I am now trying to do that following your suggestions in the post
Mesh quality criterion and best practice for generating mesh - MFiX - NETL Flow Science Software Support
Also, I made the mesh a little coarser (80x160x80) instead of the 100x200x100 mesh I was using before.
I will keep you posted on Monday.
Thanks and Regards,
Debashis
tube-cup-together-flow-only_2025-11-09T154242.472091.zip (182.1 MB)
Dr. Dietiker,
Some updates on my end.
The change in meshing (from 100x200x100 to 80x160x80) extended the run time but it still blew up. I am attaching the Zipped file (complete), the mesh stats (current tolerances) and error screenshot.
I will now try to change the tolerances and see if that helps. I have a feeling this error is related to mesh.
I will let you know by tomorrow if the changes in tolerances made any difference. I will follow your guidance (previous post) in changing the tolerance and let you know.
In the meantime, if you notice some error / mistake in the model set up, please let me know. Once I establish the single-phase flow, I need to then introduce particles.
Thanks, and Best Regards,
Sincerely,
Debashis
You need to inspect the mesh. If you did, you would see there are holes which indicate issues in the mesh:
This can usually be fixed by adjusting some meshing tolerances. Here is what I did tp get a better mesh:
- Increase the snap tolerance. This helps avoid small cut cells.
- Decrease the intersection and dot product tolerances.
- Increase the wall distance tolerance.
- Increase the domain size in the z-direction.
After that I also changed some numerical setings:
- Set norm_g=0 to relax the convergence criteria.
- Switch to first order discretization scheme.
- Increased max number of iterations for pressure and velocity.
- Increased max velocity factor.
Remember to use the xmin, xmax etc whenever possible when defining regions. You should almost never modify the Background region with hard-coded values, keep the xmin, xmax etc settings so you can change the domain extent without having to manually edit the region.
This runs fine in serial but you should consider running this in parallel (DMP) on a linux cluster.
Please try the attached:
tube-cup-together-flow-only_2025-11-10T082431.311071.zip (940.4 KB)
Dr. Dietiker,
Thank you so much. I am so grateful to you for your help and suggestions. It is running on my Windows cluster.
Unfortunately, I do not have a Linux cluster on my end. I can develop the model and run in other division’s Linux Cluster. Our group has a high-performance single Windows Machine with 88 processors for carrying out the simulations with Intel Xeon Gold 6152 processors. The machine is solely dedicated to MFiX simulations. I can use other group’s Linux Cluster to run though using the script file you uploaded.
I will keep you posted how it goes and I will also work with you to put particles inside the cup. Ultimately, I need to simulate this with particles.
Thanks again for your help.
Best Regards,
Sincerely,
Debashis
Dr. Dietiker,
Just wanted to let you know that this is running. I am trying to put particles now and will keep you posted.
Thanks and Regards,
Debashis
Dr. Dietiker,
I ran the case for 5 seconds. Attached are some plots and movie file that I created.
I will be using this .mfx file as the baseline model for implementing particles.
Any suggestion or advice in that regard from your end will be very helpful. I plan to create a box region within the cup to put particles. Similar to the DEM hopper example. Please let me know if you have any other idea on seeding the particles inside the cup.
I will keep you posted and will upload the files when I am done deveoping.
Thanks, and Best Regards
Sincerely,
Debashis
Dr. Dietiker,
I was able to successfully implement the DEM model for the particles inside the cup. It ran. I created new case “DEM-flow in cup and tube : Flow and Particle Together” and uploaded the zipped files related to the case. Kindly have a look and let me know if everything looks ok.
Also, you can mark this current case of single-phase flow Unable to run MFiX case : Single body single-phase flow as resolved.
My next messages will be in DEM-flow in cup and tube: Flow and Particle Together case.
Thanks, and Best Regards,
Sincerely,
Debashis
