hello developer
I’m doing a polysilicon fluidized bed simulation, and I want the wall to transfer heat to the fluidized bed, and it doesn’t work. The temperature in the bed keeps decreasing until it is less than the minimum temperature, and the reaction stops. I hope someone can check it out for me, thanks.
3.4.1hopper.zip (42.8 MB)
This is identical to the question
posted by user @xlli - are you the same person? or working together?
I am very sorry for the trouble caused to you. The registration failed before, so I used someone else’s account to ask questions. Now this account has just been successfully registered.In addition, could you help me solve this problem? It has been bothering me for a long time. Thank you
From your files, it looks like you have Fortran files in the project directory (usr_rates.f, etc) but are using the default MFiX solver. If you have reacting chemistry, you must build and use a custom solver. See section 5.1 of the MFiX user guide for more information.
You should have seen a warning popup like this
Was it displayed?
Yes, it has shows.Sorry, I didn’t know that there was a chemical reaction that required the creation of a solver. However, now that I’ve successfully built the solver, it doesn’t seem to be converging again.
3.4.1hopper.zip (56.5 MB)
Instead of zipping up the entire project directory, use “submit bug report” and upload the ZIP file that is created. The ZIP files you are uploading contain a lot of extra data we don’t need.
It didn’t error out yet, but I ran it for 4 hours and it didn’t start calculating, so I paused it. This is a bug report.
hopper3_2023-07-27T094831.687319.zip (10.6 MB)
I ran the simulation for about 16 hours and it did not crash - it just runs extremely slowly.
At the current rate, it will require about 90 days to complete. It seems to be spending a lot of time in the chemistry part of the solver - note the large number of messages starting with DLSODA - these all pertain to the stiff solver.
Things to try:
- Run on more cores (DMP)
- Disable the stiff chemistry solver - according to Sec 4.13.6.2 of the MFiX manual the stiff solver may make simulations run faster or slower, depending on the reactions.
- Adjust the maximum number of substeps for stiff solver (
stiff_chem_max_steps) - Simplify the chemistry
First of all, thank you very much for your help, through your third suggestion this case can be run. However, the problem is back to the beginning, I was hoping to transfer heat through the wall but it doesn’t seem to work, the temperature keeps dropping. I checked the help document and saw that STL is an invalid boundary condition. Is it because the wall does not conduct heat because the wall is an STL area?Or other reasons?
hopper3_2023-07-31T095539.034002.zip (70.5 MB)
Ok, we have a few issues here:
- I cannot compile your project from the .ZIP file uploaded. I’m getting the error:
Fatal Error: Cannot open included file usrnlst.inc
Do you have usrnlst.inc in your project dir? Can you upload it?
- The section of the manual you quoted is in error
Note that the MFiX GUI will not allow you to select inappropriate region types.
Here’s the section of the MFiX spec where this is spelled out:
-
Select boundary type
-
Selection is required
-
Available selections:
-
Mass Inflow
- Plane regions set keyword BC_TYPE(#) to ‘MI’
- STL regions set keyword BC_TYPE(#) to ‘CG_MI’
- Not available for volume regions
-
Pressure Outflow
- Plane regions set keyword BC_TYPE(#) to ‘PO’
- STL regions set keyword BC_TYPE(#) to ‘CG_PO’
- Not available for volume regions
-
No Slip Wall
- Volume and plane regions set keyword BC_TYPE(#) to ‘NSW’
- STL regions set keyword BC_TYPE(#) to ‘CG_NSW’
-
Free Slip Wall
- Volume and plane regions set keyword BC_TYPE(#) to ‘FSW’
- STL regions set keyword BC_TYPE(#) to ‘CG_FSW’
-
Partial Slip Wall
- Volume and plane regions set keyword BC_TYPE(#) to ‘PSW’
- STL regions set keyword BC_TYPE(#) to ‘CG_PSW’
-
Mixed Walls
- Volume and plane regions set keyword BC_TYPE(#) to ‘PSW’
- STL regions set keyword BC_TYPE(#) to ‘CG_PSW’
-
Pressure Inflow
- Plane regions set keyword BC_TYPE(#) to ‘PI’
- Not available for volume regions (note ‘CG_PI’ does not exist)
- Not available for STL regions
-
Mass Outflow
- Plane regions set keyword BC_TYPE(#) to ‘MO’
- STL regions set keyword BC_TYPE(#) to ‘CG_MO’
- Not available for volume regions
-
Cyclic
- No region to select
-
-
Yes, i have usrnlst.inc in my project and i can upload it. But it is not in the bug report, it is in the project file.I re-uploaded the project file. Please help me to see the reason for the temperature drop. Thanks.
3.4.1hopper.zip (45.8 MB)
Sorry, our team has been very busy and we haven’t had a chance to look into this yet. I’ll try to take a look at it this week.
I haven’t gotten to the bottom of this but I can confirm the temperature drop. It’s happening at the outlet. The wall temperature and initial bed temperature is set to 923K, but the material coming in the inlet is 473K, so a temperature drop in the bed is expected. But I don’t understand what’s going on at the outlet. The outlet temperature is set in the BCs to 923K.
For debugging purposes, I suggest:
A) Disable all chemical reactions. This will make the simulation go faster and the problem does not seem related to chemistry (the plot above is from a run with chemistry disabled)
B) Increase the write frequency for monitors. This will allow you to see the temperature drop in the plot without waiting as long.
I will follow up when I know more.
– Charles
You are running a pseudo-2D simulation: 3D mesh with only one cell in the z-direction. You need to set the BCs along the front and back boundaries.
1 Like
OK, thank you very much.
Thanks for your advice, after I set the BC on the front and back, the temperature did not drop anymore. However, I have a question: the front and back boundary condition I set is No-silp wall, but in the real reaction, there is no wall resistance in front and back. Is there a more suitable boundary condition?
An adiabatic free-slip wall may be more appropriate here.
OK, thank you very much.