HI @jeff.dietiker @cgw I am working on TFM modelling and I have been facing convergence error. The solution converged for 0.02 seconds and then Dt<dtmin error emerged. I have run the same geometry in DEM modelling, with similar particle size and similar mesh cells and the solution converged for whole 5 seconds. yet, it does not run in TFM. I am sure somewhere in the setup there ought to be certain changes.
- I have solved the wall issue in the loop seal as suggested by you and the mesh looks perfect now.
I have seen your replies concerning a similar issue other users are facing and i am jotting down the solutions you provided. Can you please provide me a deeper insight if a similar solution is applicable to my problem.
- 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).
- 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).
I need help with this. Please provide me your suggestions.
INLETASSWITHCYCLONE.msh (12.2 MB)
inletasswithcyclone.mfx (10.7 KB)
Please attach your stl file.
@jeff.dietiker the files are big. how do I attach a large file?
Hello @jeff.dietiker , I have made few additional changes to the setup.
- reduced default tolerance (tol_resid) of 1E-4
- increase the number of gas pressure equations to 200 (Numerics>Linear solver)
3.decrease the initial solids volume fraction (Initial Condition>Bed>Solid 1 tab)
and the simulation has begun. If i find the solution is still not converging, I will post the files again.
Hello @jeff.dietiker @cgw , I have tried almost every solution i could think to improve convergence, but the simulation runs for some milliseconds and diverge. Now i really need help with understanding the problem to this issue.
Can you please help me resolve it? I am stuck now
https://sooners-my.sharepoint.com/:f:/g/personal/sayyamchopra_ou_edu/Eo_R6qIQp39Dnw2nX4TDYwkBSgRpbbI6RZoIggDv-1exig?e=L4lDa2
The mesh in the loopseal is not good. You will need to refine the mesh. But first, you should re-export the stl file, it is way too large (400+ MB). You don’t need that many facets with such a coarse mesh.
Hello @jeff, i used a recommended approach to use mess cell size =10 times particles size. What do you suggest about it ?
Sure, I will check why my STL file is too large.
thanks , I will try your solution and confirm regrading this issue, If the issue is resolved or not.
The mesh needs to resolve the gap between the walls in the loopseal. You could refine by a factor of 2 in each direction.
The wall looks odd (see region highlighted in red below). Is this intentional?
No @jeff.dietiker , its not intentional. I think it due to poor cell size I have chosen. Factor of 2 means, i can increase the cells by a factor of two. Is it?
I have tried to improve the mesh for 0.0005mm particles. do you think this is alright ? Or do i need to make any changes because i see it hasn’t improved a lot.
This is the STL file, not the mesh. My guess is you want the wall geometry to be cylindrical in this region. First, clean the geometry, and export the stl file so it is manageable. You don’t need more than 50,000 triangles for this geometry (You currently have 8.5 millions triangles). Then you can play with the mesh parameter. Your current mesh is 65x155x16 cells. Refining by a factor of two means 130x310x32 (twice as many cells in each direction).
sure @jeff.dietiker , I will update you. I made the geometry in ansys and it look perfectly cylindrical. Yet, Let me see if i could refine it.
But, when you say refine by a factor of 2, then i couldn’t use the 0.0005mm particle size because it would follow the 10 times the particle size criteria. then i need to change the particle size as well.
I am a little confused, sorry.
You will hear people say the grid size should be around or less than 10 particle diameters, this is just a rough guidance, you don’t need to have the grid size locked to exactly 10 particle diameters. Keep the particle size you want to model and vary the grid spacing until you have a decent mesh.
Thanks @jeff.dietiker , I will make changes suggested by you and keep you updated if i have any more concerns.
Hello @jeff.dietiker, I have followed your guidelines and suggestions, yet the issues still persist. If you have some time, Could you please check if my setup is fine or not?
I think this new mesh which I set up with a factor of two seems to be fine, yet, there still exists some issues which I couldn’t understand. Also, I have tried my best to refine the mesh but i could not understand if the problem is with the mesh or setup.
Please help me if you have some time. I am stuck on this issue and due to this, I am not able to complete my research paper.I have results in DEM, but I am stuck on Eulerian modeling.
Thank you
INLET ASSM WITH BEND AND CYCLONE1.stl (276.5 KB)
geometry.stl (455.2 KB)
geometry.stl (455.2 KB)
CYCLONE1_FACETS_READ.stl (649.2 KB)
BOX1_FACETS_IGNORED.stl (25 Bytes)
cyclone1.mfx (10.5 KB)
Please try with the attached. I increased the number of iterations for pressure and velocity. I also increased the mesh tolerance for wall distance. You are using a finer mesh than I suggested, this may run too slow for you, and you can coarsen the mesh a bit.
cyclone1.mfx (12.4 KB)
Hello @jeff.dietiker ,
Firstly, thanks a lot for being prompt to answer my queries. I am glad you have always been a great help to me.
-
So, if you had to conclude, was the issue in the setup or mesh, or was it a combination of both? I really need to understand this.
-
When you suggest coarsening the mesh, you indicate reducing the no of cells in the X/Y/Z direction. Is it? or is it playing with mesh parameters like (small cell tolerance ) or other parameters?
-
How did you increase the mesh tolerance for wall distance?
-
So, can I conclude that in TFM modeling, the mesh needs to be perfect and then I can input any size of the particles without worrying about the basic thumb rule that is cell size=10 times particle size? Can it be concluded?
Also, since according to you my mesh is very fine, I will coarsen the mesh once I get an understanding from you of what coarsening the mesh means.
Right now, as you said, my simulation is too slow. Also, can you tell me for this kind of simulation is better, DPM or SMP approach? I have a 64-core CPU and I purchased it only for this kind of simulation.
- I think it was a combination of both. There was some high velocity due to bad mesh and a lack of convergence (after the mesh improved) due to small max number of iterations foe pressure equation. You can also try to switch to ideal gas law see if it converges better.
- I am suggesting reducing the number of cells in each direction, based on your current setup. The setup you sent is finer than I what I initially suggested. Original mesh=65x155x16, I suggested 130x310x32, and you sent 160x376x40. you could use 130x310x32 or somewhere between 65x155x16 and 130x310x32.
- Mesh>Mesher pane, set the normal distance tolerance to 0.01 (tol_delh)
- There is no perfect mesh in CFD. You have to trade between speed and accuracy. You want to use the finest mesh you can afford. Ideally you would want to do a grid refinement study (see how far you can refine the mesh until results are insensitive to the mesh). This is difficult to do in practice. If the mesh becomes too coarse (say 100 particle diameter), then you will miss features in the flow.
I would say DMP will be faster.
@jeff.dietiker
I am glad you shared such a piece of valuable information with me. Thanks a lot for your time and all the suggestions. Soon after this simulation is done, I am planning to put the whole chemical looping geometry for the run and I hope all these suggestions would work.
Again, thanks for guiding me through.
Also, one more query, If you say that DMP would be faster, what do you recommend if I have 64 cores? Can I know your ideal breakup of the cores?
Thanks
Sayyam
I would say a 2x8x4. Here you want to use as many cores in the z-direction as possible, but there are not that many cells in the z-direction. x and y direction will be unbalanced due to the geometry.
