HI, I AM WORKING ON CHEMICAL LOOPING REACTOR DESIGN AND I AM TRYING TO IMPLEMENT TFM MODELLING. I DO NOT UNDERSTAND WHY AM I GETTING (DT < DT MIN) ERROR.
CAN SOMEONE PLEASE HELP ME OUT TO UNDERSTAND THE REASON BEHIND THIS ERROR?
I KNOW THE Dt < Dt min ERROR OCCURS WHEN WE HAVE ISSUE RELATED TO GEOMETRY, BOUNDARY CONDITIONS AND CONVERGENCE ISSUE. I HAVE CROSS CHECKED AND VERIFIED EVERYTHING AND YET THIS ERROR IS CONTINUOUS.
I NEED PROFESSIONAL HELP TO UNDERSTAND THIS ISSUE. ALSO, I WOULD BE GLAD IF SOMEONE COULD OPEN MY FILE AND TRY TO UNDERSTAND.
geometry_0001.stl (4.5 MB)
geometry_0005.stl (3.7 MB)
stlmainchemloop.mfx (18.3 KB)
STLMAINCHEMLOOP.msh (18.6 MB)
STLMAINCHEMLOOP_FACETS_READ.stl (6.0 MB)
Did you solve your convergence issue? I see you have other postings with post-processing questions.
Hello Jeff, I am not able to figure out the reason behind the convergence issue ? Could you or any team member help ,e figure out the reason? I have tried almost everything to understand the reason behind convergence. The same model works for DEM modelling but not for TFM.
Yes, i have several other post processing questions based on the same simulation, but i have posted it as a different query because it would help me understand individual topic better.
The walls in the loopseal and cyclone vortex finder are too thin compared with the mesh size. You will need to refine the mesh and probably increase the thickness of the walls so they can be resolved.
Hello Jeff, thanks for the reply. Can you please explain me or guide me about how to improve meshing or refine the mesh (as you stated)?
Also, how do i increase the thickness of the wall? As you design the geometry, we make solid cylinder body and unite them together. So, there isn’t any thickness involved in the system as it is a solid geometry.
I have been trying very hard to solve this issue. Please guide me through this as i need to produce the results and i cannot produce since a very long time.
Jeff, i am attaching screenshots of the mesh i have used recently. Can you please tell me if i could reduce the cell size beyond this? It is because my particle size is 4mm and most of my cell in I/J/K cells have cell size close to 4mm. If i go below this, the simulation shows a convergence error in the very beginning.
Through these screenshot , can you please explain me how do i refine mesh and is it the right approach i am following?
I am replying here but this will also apply to your previous post. The grid spacing (visualized as the blue mesh above) must be finer that the smallest geometric element you want to resolve. Here I think the smallest is the internal wall in the cyclone and loopseal. If you lower the opacity of the stl file, you may be able to see that the mesh is too coarse. You wan to get more than one cell within the internal wall gap, otherwise you will end up with bad cut cells. You can start by refining the mesh, but this may not be sufficient since there is also a constrain of the cell being larger than the particle diameter. If this is not sufficient, you can artificially increase the wall thickness until you can resolve it. This means generating a new STL file.
Please take a look at 3.21. SMS meshing workflow, cyclone, Discrete Element Model (DEM) — MFiX 22.2 documentation for an example to inspect and improve the mesh.
thanks Jeff. I understand few parts of what you wanted to convey. Yet, can you please clarify the issue related to WALL THICKNESS? I do not understand how to increase the wall thickness and which wall thickness are you talking about?
When I make geometry in ANSYS, it does not consider any wall thickness because I use solid cylinders and unite then together. May be i am not clear with the concept of wall thickness.
Also, I have already seen the tutorial file and i have tried almost everything. How do you suggest improve the mesh?
thanks for all your suggestion but can you please elaborate your suggestions?
What I call the wall thickness is the gap between the two cylinders (in red below). The grid spacing (in blue) is much larger than the wall thickness so you cannot resolve it.
If you look at the mesh, you will see that the vortex finder is not fully resolved due to missed intersections. There are also some holes in the mesh as a consequence.
You need to refine the mesh (increase the number of cells in each direction) and increase the wall thickness, by going back into ANSYS and redoing the geometry with a larger gap (change the radii of the cylinders).
thanks a lot Jeff. Now i completely understand what you meant by grid cell and wall gap. a great help indeed.
Yet, One last query from me " How did you generate the second image you sent me?" The one in which the solid body has mesh on it. I know how to generate the first pic, but not the second one. Please help me with one last query. Also, i will try to apply your solution and let you know the progress.
I know its from the bar on the right on the GUI. I think i have to go to mesh and click reload. But, can you please tell me how did you get such a transparent geometry with properly seen geometry?
You can toggle the visibility of each item by clicking on the icons next to the their names. Here I am only showing the boundary mesh (the geometry, background mesh, and regions are hidden) and lowered the opacity to see the internals. I did not load the full 3D mesh so it is not showing.
fluid_bed_tfm_2d.mfx (8.5 KB)
Hello @jeff.dietiker I am facing the following error in 2D Two Fluid Model:
ERROR from time_step.f:193
DT < DT_MIN. Recovery not possible!
Fatal error reported on one or more processes. The .LOG file
may contain additional information about the failure.
Please go through it once and help me resolve it.
Either decrease the initial solids volume fraction (Initial Condition>Bed>Solid 1 tab) or decrease the solids fraction at onset of friction (solids>TFM tab).
Hello @jeff.dietiker . I am trying to simulate a 2D bi-disperse fluidized bed using two fluid model. I have attached the images of model geometry and parameters to this reply. When the specified inlet velocity is below 11 cm/s, solution diverges and an error message saying Dt<Dt_min pops up which automatically terminates the simulation. I am facing this convergence issue for only low inlet gas velocities (<0.11 m/s), otherwise it works fine.
Please help me resolve this issue.
How soon does it diverge and are you below minimum fluidization velocity? You can try to start with some non-zero initial velocity in the vertical direction.
If you get stuck, please attach your simulation file.
Hello Jeff. Please find the attached MFX file. Thanks in advance
TFM_finemesh_bidisperse_LBST_0.02975.mfx (11.3 KB)
My guess is you are below minimum fluidization velocity. You start with a packed bed so there is not much to make the solution change. Your pressure residual is already small (1E-10).
Here you should not set the DT factor to 1, set it to 0.9. If you want to use constant fluid density, try increasing the number of iterations for the pressure equation (Numeric>Linear solver pane). You can also change the fluid normalization to 0.0 (Numerics>Residuals).
Earlier the time step factor was 0.9. I changed it to 1.0 to overcome the initial nonconvergence. I will try to incorporate your suggestions.
Edit - Thanks a lot. It helped.