Hello everyone,
I am writing this because I am trying to model a dual circulating bed system using the TFM approach and I am having significant problems in attempting to run the simulation. I have tried to upload the geometry of the beds as an external stl file that I produced using Freecad (see the file named riser only) and as geometry using the available Mfix procedural curves (see file riser_mfix_geom) but the simulation keeps failing in both cases and I don’t know how to fix it (as of now, the error it gives is DT<DT_MIN, I have tried changing DT_MIN, or refining the mesh, but it does not appear to work). Furthermore, the file with MFIX preavailable geometries as since stopped working completely: it starts the run, but it is immediately stopped without even producing the mesh, but it does not give any errors. My final plan was to simulate the whole dual bed system using the stl file I made, but so far I have been unsuccessful, even in modeling only part of the apparatus. I need at least the riser results to compare them to experimental data. Please, can anybody help me to understand what is wrong with my simulation attempts? I am completely new to this kind of work and I don’t know what I can do.
The .mfx file in Riser_only.zip needs cyrcil_new.stl which is not included in the zip file. Is this the same as cyrculating complete.stl?
If you want better support please make sure you include all files necessary to reproduce the error. It is best to use the built-in feature to generate a zip file. Go to the main menu, select “Submit bug report”. This will generate a zip file that you can attach here.
Here is the ZIP of the new simulation attempt I made. The bug report feature of MFiX does not apper to be working properly unfortunately, it runs for a lot of time without completing the folder.
With that said, I had to use a rather fine mesh in the simulation because otherwise it would not get the stl file right. Right now it always gives problems with solid and gas velocity and I don’t know why. To explain what I am currently trying to do: in the gasifier, I am simulating a bed of fine particles, while from one of the pipes at the top of the bed, coarser particles representing biomass are injected. The fine particle should circulate from the gasifier to the riser from the siphon, then be entrained, separated by the cyclone at the top of the riser and reintroduced in the gasifier from the top. I produced the stl file for bed geometry in FREECad software. I tried altering the mesh and the boundary conditions, but I can’t manage to get the simulation to run. Did I set the boundary conditions in the wrong way? I planned to implement also the combustion reaction but first I wanted to get the fluid dynamics to work.
You have some extremely large aspect ratio (see MESH_STATS.LOG or the MESH STAT pane):
============================================================================
HISTOGRAM FOR: Aspect Ratio (SCALAR CUT CELLS)
MIN = 0.1005E+01
MAX = 0.1997E+04
============================================================================
0.100E+01 --> 0.201E+03 |######################## | 48093 CELLS OR 98.9%
0.201E+03 --> 0.400E+03 | | 331 CELLS OR 0.7%
0.400E+03 --> 0.600E+03 | | 121 CELLS OR 0.2%
0.600E+03 --> 0.799E+03 | | 55 CELLS OR 0.1%
0.799E+03 --> 0.999E+03 | | 18 CELLS OR 0.0%
0.999E+03 --> 0.120E+04 | | 7 CELLS OR 0.0%
0.120E+04 --> 0.140E+04 | | 3 CELLS OR 0.0%
0.140E+04 --> 0.160E+04 | | 3 CELLS OR 0.0%
0.160E+04 --> 0.180E+04 | | 0 CELLS OR 0.0%
0.180E+04 --> 0.200E+04 | | 2 CELLS OR 0.0%
============================================================================
You will need to increase the small cut cell tolerance and the snap tolerance until it is reasonable.
There are some fairly thin walls or gaps than need a very fine mesh. My suggestion is you start with a simpler geometry, maybe just one component of the gasifier, or remove all small internal walls (vortex finder) that make the meshing challenging. If you can get this to run, then you can try to add some complexity one step at ta time.
I tried not working with my .stl file, here are two attempts at modeling only the gasifier using the implicit geometry (file cyl_1) and procedural geometry (file proceduralgeometry). I also temporarily removed the solid inlet from above (the cyclone) and the syphon connecting the beds. It still does not work. If I limit the y axis to include only the main gasifier cylinder, the simulation runs but is incredibly slow. As soon as I try to incorporate the upper conical part of the bed, it starts running for ages without ever completing the first time step. I removed everything except the gasifier cylinder and the small cylinder output, it shouldn’t be a difficult geometry, yet it still does not manage to work even with the inbuilt geometries. The aspect ratio did not seem to be so bad, what else could be wrong?
Increase the snap tolerance (say 0.05). Mesh>Mesher pane.
Increase the normal distance tolerance (say 0.05). Mesh>Mesher pane.
Switch to ideal gas. If you want to use incompressible fluid, increase the linear solver iterations for gas pressure (say 200) and gas velocity (say 50). Numerics> Linear solver pane.
Use a fluid normalization of 0 (Norm_g in Numerics>Residuals pane).
Decrease the initial solids fraction, you are at max packing.