Mfix-19.3.1 run issue

[jagan1mohan]

Hi @cgw, here is zip file that is generated after clicking “Run” on GUI on laptop. Could you please help me here?

umf_500_2500_10x_5p0y_2022-02-21T151941.595290.zip (31.8 KB)

Best,

[jagan1mohan]

@cgw, here is output from “conda list” after issuing “conda activate mfix-19.3.1”

condaList.txt (7.6 KB)

Best,

[cgw]

Hi Jagan.

Just to be clear, it looks like there are two separate issues now? You can’t run at all on your laptop, but you got MFiX running on a cluster… but the results on the cluster are different from what you expected - is that correct?

A few points:

1. I see that you are running MFiX version 19.3.1. If possible, please upgrade to version 21.4. It is difficult for us to find and fix bugs in older versions, especially if those bugs are not easily reproducible. If this bug is still present in the current version, we will investigate further.

2. Your report starts with “Could not import VTK”, but the traceback was omitted. That information can be helpful for debugging. Sometimes VTK issues are due to older hardware not supporting modern GL shaders, which newer versions of VTK require. If you are installing on an old laptop you may need to use something like “vglrun”

3. Will follow up separately regarding the cluster run.

– Charles

[jagan1mohan]

Hi @cgw, at the moment, let us focus only on local machine installation. (At least I’ll have something to use as I’m chasing a deadline).

1. I started all-over again to install latest version available which is MFiX 21.4.
   Towards end of “sh Anaconda3-2021.11-Linux-x86_64.sh” step, I see syntax error as shown.
   

   
   
   Can this be an issue?

2. After this, in a new terminal, “conda” output is as shown. I copy-paste link from MFiX downloads page.
   

   
   
   Is conda output okay?

3. Software gets into iterations without any errors. [I’d update you about results very soon].
   3a. I’d setup this version on cluster and see if this works.

4. Case I’m testing has a point probe on centroid of YMIN region. There’s a monitor “Average” type to calculate pressure and y-velocity, besides, point probe monitor.
   

   
   
   Numbers from point probe, say v_g, are close to UDF values but “Average” monitor is clearly failing. What is the issue?

Thank you.
Best,

[cgw]

Hi Jagan.

1. I have not seen this error before, but searching for Anaconda3-2021.11-Linux-x86_64.sh 516 Syntax error unexpected
   got me a few results.

https://github.com/ContinuumIO/anaconda-issues/issues/12809

installation - Can't install anaconda on Ubuntu 20.04. ~/anaconda3 folder is not created? - Stack Overflow

These both point to permissions problems, ie using sudo to install. Since this is not an MFiX-specific problem I’m afraid I can’t provide further insight on this one. It may not even be a problem (?)

2. conda output looks fine. But in the second screenshot, I see the message To launch MFIX: MFIX
   This is not coming from our installation, this must have been added by someone at your university who previously installed MFiX. I can’t guarantee that your installation and this installation are not going to interfere, you may have to get help from a local systems person. However, if you have your own Anaconda installation activated, that should take priority over whatever is previously installed.

3. It runs! Hooray.

4. Please attach case files (“Submit bug report” from main menu) if you want us to diagnose output.

Thanks,

– Charles

[jagan1mohan]

Hello Charles @cgw, please find attached zip folder to address monitor(s) issue. I tried “Average” and “Area-Weighted Average” and both are failing as shown below.

My observation is point probe is writing superficial gas velocity at its location, which is one-cell above YMIN face and other two monitors are writing bc_v_g(1) from usr1.f
I think, to estimate UMF or for fluidization studies, superficial gas velocity is more appropriate. If we can get average across boundary instead of point probe, it is more acceptable

As a reminder, I’m using TFM on rectangular domain (please see above, no cut-cell, 2 cells thick).

      A. VTK files, say BG_0010.vtu, are saved in binary. Can it be saved as ASCII or txt or csv?
      B. How to write txt or csv table with x, y, z (of cell centroids) and pressure, voidfraction....? [I read a post where Paraview exports each vtu file into csv but I have around 400 vtu(s) to work on].

Best,

[jagan1mohan]

umf_500_2500_10x_5p0y_2022-02-28T173950.133117.zip (236.0 KB)
UMF_500_2500_10X_5p0Y.mfx (17.6 KB)
usr1.f (2.8 KB)

Thank you.

[onlyjus]

I would suggest either scripting paraview or just writing python code to read the vtu files and write the values to whatever you want:

Saving data as .csv files

I have run a DEM model in mfix and now want to save the particle data for each time step. I have seen that I can do this through importing the .pvd file into paraview and see the spreadsheet of data. However, I want to save all the velocity/coordinates of each particle for each time step. I see I have a series of .vtp files containing this information. Do i have to individually put these into paraview and save the data, or is there a way to save all the data at once?

[jagan1mohan]

Hello Team,

@onlyjus: Thank you. I’ll try this and would revert you back.
@cgw : Did you find a chance to look into my request on average monitors?

Best,

[cgw]

Not yet, Jagan, sorry.

[jeff.dietiker]

Why are you saying that “Average” and “Area-Weighted Average” are both failing? They give you the correct gas velocity (as specified in usr1.f) at y=ymin plane. This is a BC value. I am not sure what value you were expecting.

The value in BOTPOINT.csv is not superficial velocity, it is just the gas velocity at one point in the flow field. It won’t be the same as the BC value.

[jagan1mohan]

Hello Dr. @jeff.dietiker, thanks for your reply. Could you please find the attached slide for more information on my question?

Questions:

1. Can a 2 mm distance (between YMIN AVERAGE and POINT PROBE) has this different gas velocity?
2. If YMIN AVERAGE is working correct, why pressure is always 101320, when bed is vigorously bubbling?
3. Zero pressure drop across bed as this is PressureOutflow value?

Best,

[jagan1mohan]

Also attaching, void fraction field, for first few seconds, for your reference.

Best,

[jeff.dietiker]

1. Can a 2 mm distance (between YMIN AVERAGE and POINT PROBE) has this different gas velocity?

Yes. Again, you should not compare the inlet velocity (where void fraction is one) with the gas velocity in the bed (where the void fraction is less than one). For example if the inlet velocity is 0.7m/s and the void fraction in the bed is 0.5, then the gas velocity at that point won’t be 0.7m/s but close to 0.7/0.5=1.4 m/s due to the volume occupied by solids.

2. If YMIN AVERAGE is working correct, why pressure is always 101320, when bed is vigorously bubbling?
   YMIN AVERAGE gives you the velocity at y=ymin, but it correspond to the ghost cell just below y=ymin because the y-velocity is stored at the north face of the cell (staggered grid representation). The pressure is stored at the cell center. The value 101320 is not applied but used to compute gas density. The pressure you want to use for a pressure drop calculation is the pressure at the first fluid cell above the inlet and the pressure at the outlet (outflow pressure).

3. Zero pressure drop across bed as this is PressureOutflow value?
   See answer to 2)

[jagan1mohan]

Dear Dr.@jeff.dietiker, thank you for your quick reply.

A. It is interesting to note that void fraction at YMIN plane is always 1.0. This confirms that imposed boundary condition value, bc_v_g(1), in GUI or UDF, is superficial gas velocity of system.

Also, this value being a constant, in my case, it is uniform across entire patch / boundary. So, average/value type(s) monitor is same.

B. How can we output an average of pressures at all first fluid cells above inlet? If I understood staggered cell arrangement correctly, red line shows the plane where this pressure is to be evaluated for pressure-drop-curve. Please see attached image below and ignore probe representation in this figure.

Best,

[jagan1mohan]

And (this pressure minus 101320) versus superficial gas velocity, show allow us to calculate minimum fluidization velocity of the system.

[jagan1mohan]

Hello Dr.@jeff.dietiker, @cgw, @onlyjus, I think, I figured out procedure to extract pressure-drop across bed.

1. I created a plane above YMIN (gas inlet) such that its position is around 75% of first-cell-height. For lower positions, say 50% or 25%, average-pressure-monitor showed e+32 garbage values.
2. With superficial gas velocities directly obtained from usr1.f, we see following plots.
   
   
   
   In my opinion, minimum fluidization velocity is 0.316 m/s, occurs at 11.57s from start. Could you please confirm this data extraction from MFiX is correct?
   Best,

[onlyjus]

IMO, if you are just trying to get minimum fluidization velocity, then it doesn’t matter where in the bed you are measuring the pressure. All you need is a pressure vs superficial gas velocity curve. Of course, it is nice to see the bed “weight” in the pressure (more so from the experimental side to verify that the bed mass/pressure/location are all consistent).

Anyway, looks like a nice Umf curve to me.

[jeff.dietiker]

Looks good to me. As Justin said, some people like to normalize the pressure drop by the weight of the bed so the plateau has a value of one.

[jagan1mohan]

Thank you, Dr.@jeff.dietiker, @onlyjus for your confirmation. I think, now I understood umf extraction from MFiX setup.

→ My observation is particle volume fraction is 0.58 when gas velocity approaches zero in above simulation. This value, I confirmed for few other particle types also.
A. Can we say, in TFM, maximum particle volume fraction is 0.58?
B. In setup initialization, I used particle volume fraction as 0.55 (guess) and perhaps, more correct value is 0.58?

→ For parallelization, is there a “most probable” optimum nCells / CPU based on your experience, for best speed-up? We know, too many or too less CPUs kills speed. There are no cut-cells here.

→ Output file shows that choice of parallelization is OpenMP. I believe, I have access to MPI on cluster, is this better than OpenMP?
ENABLE_MPI = OFF
ENABLE_OpenMP = 1
ENABLE_NETCDF = OFF
ENABLE_CTEST = OFF
ENABLE_COVERAGE = OFF

Best,