Post Processing
===============
MFiX can generate output data in several formats for visualization and analysis.
The command line tool ``postmfix`` is distributed with MFiX. In addition, the
MFiX output file format is supported by the open source GUI tools `ParaView
<https://www.paraview.org>`_ (version 4.1 or later) and `VisIt
<https://wci.llnl.gov/simulation/computer-codes/visit/>`_.
The following table lists the files typically associated with an MFiX simulation.
.. include:: /output_format_table.rst
Notes:
1. pvd files only contain information linking the respective .vtu and .vtp files to time- step information.
2. <VTK_REGION >_###.vtp files are binary files. The <RUN_NAME >_DES_###.vtp are ASCII files.
Running ParaView
~~~~~~~~~~~~~~~~
This walk through demonstrates how to use ParaView to visualize the results of
the `dem/fluid_bed_2d` tutorial. It is assumed that the `dem/fluid_bed_2d` tutorial was
successfully run with default settings and that ParaView is installed on your
system. First, the tutorial demonstrates how to visualize the fluid field; then,
the DEM particles are added using spherical glyphs.
.. role:: u
.. _fig_paraview-fileopen:
.. figure:: /media/paraview_1.png
:figwidth: 8cm
:width: 8cm
:alt: paraview visualization
Click on File icon |file|, or :u:`F`\ ile > Open
Fluid field results for a standard structured mesh are displayed in ParaView by
loading the .RES file. To open the RES file, click on File/Open
(:numref:`fig_paraview-fileopen`), and navigate to your run directory.
Select the ``DES_FB1.RES`` file (:numref:`fig_paraview-loadres`).
Do NOT load the DES restart file (``DES_FB1_DES.RES``). This binary file is not
supported by any visualization software. It only contains restart data and will
likely cause ParaView to crash if loaded.
Once the file is loaded, you need to click on the green "Apply" icon |apply| to load
all of the variables.
.. _fig_paraview-loadres:
.. figure:: /media/paraview_2.png
:figwidth: 8cm
:width: 8cm
:alt: paraview visualization
Load ``DES_FB1.RES`` (do NOT load ``DES_FB1_DES.RES``)
Newer versions of ParaView require that you select the appropriate reader.
Choose to open the data with "MFiX Unstructured Grid Files".
(:numref:`fig_paraview-unstructured`)
.. _fig_paraview-unstructured:
.. figure:: /media/paraview_3.png
:figwidth: 8cm
:width: 8cm
:alt: paraview visualization
Select "MFiX Unstructured Grid Files"
ParaView typically displays the gas phase volume fraction once the data is
loaded. It may be necessary to rescale the data range as the initial range may
only be suitable for displaying the initial conditions. This can be done by
clicking the |rescale| icon.
.. _fig_paraview-pvd:
.. figure:: /media/paraview_4.png
:figwidth: 8cm
:width: 8cm
:alt: paraview visualization
Open DES_FB1_DES.pvd
DEM and PIC particle simulation data is loaded into ParaView by opening the
``.pvd`` file. (:numref:`fig_paraview-pvd`)
Again, click on the green "Apply" icon |apply| to load all of the variables.
(:numref:`fig_paraview-load`)
.. _fig_paraview-load:
.. figure:: /media/paraview_5.jpg
:figwidth: 8cm
:width: 8cm
:alt: paraview visualization
Load all variables
Particles are shown by applying a glyph to the
dataset. To apply a glyph filter, either:
- :u:`F`\ ilters > Alphabetical > Glyph
- or click the |glyph| icon.
Commonly, particle data is represented using:
1. `Sphere` glyph type and
2. Scalar scale mode with a scale factor of one.
Note that these screenshots may appear differently depending on your version of
ParaView.
.. |apply| image:: /media/paraview_apply_icon.jpg
:width: 1cm
.. |file| image:: /media/paraview_file_icon.png
.. |glyph| image:: /media/paraview_glyph_icon.jpg
.. |rescale| image:: /media/paraview_rescale_icon.jpg
Building postmfix
~~~~~~~~~~~~~~~~~
The ``postmfix`` command is used for reading the binary MFiX ``.SPx`` output
files and outputting data to text files. The following walk-through demonstrates
how to run ``postmfix`` on the results from the `dem/fluid_bed_2d` tutorial with the
default settings.
The ``postmfix`` executable is built by running ``build_mfixsolver`` with the
``--postmfix`` flag:
From the installed package:
.. substitution-code-block:: shell-session
(mfix-|release|)$ build_mfixsolver --postmfix
From source:
.. substitution-code-block:: shell-session
$ cd mfix-|version|
$ mkdir build
$ cd build/
$ cmake .. -DENABLE_POSTMFIX=1
$ make postmfix
Running postmfix
~~~~~~~~~~~~~~~~
After building, run the executable and enter the run name:
.. substitution-code-block:: shell-session
$ ./postmfix
Enter the RUN_NAME to post_process > DES_FB1 ? DES_FB1<Enter>
A simple menu of options is presented. Type `1` to examine/print data and press Enter.
.. code-block:: shell-session
*************************************************
0 - Exit POSTMFIX
1 - Examine/print data
2 - Write .RES from data in .SPx files
3 - Write .RES for a new grid, using old data
4 - Calculate miscellaneous quantities
5 - Print out variables
6 - Call user defined subroutine USR_POST
7 - Write a new SPx file with selected records
8 - Write new SPx files with time averaged data
9 - Perform ORNL calculations
10 - run scavenger code
*********************************** **************
Enter menu selection > 1
Interactive data retrieval program. Type ? any time for help,
or press RETURN to select default values shown in parenthesis.
Type F to use the default data precision and press Enter.
.. code-block:: shell-session
Write output using user - supplied precision? (T/F) F ? F<Enter>
Enter a time range for data extraction and analysis. The default simulation has
a simulation length of one second, so enter a range from 0.1 seconds to 0.9
seconds. The next prompt asks if the data should be time averaged. Press Enter
to skip the averaging.
.. code-block:: shell-session
Time: (0.000, 0.000) > 0.1, 0.9
Time average ? (N) > ? < Enter >
Enter the variable of interest. The default is the gas phase volume fraction,
EP_G. A complete list of possible entries is given by typing `?` and
Enter. Press Enter to select the gas phase volume fraction.
.. code-block:: shell-session
Variable: (EP_g) > ? < Enter >
Next, enter the spatial range to extract the data. This requires an understanding
of the I/J/K values for your simulation. Basic geometric information for the
simulation is provided in the .OUT file. For this example, we will take a
vertical slice from the approximate center of the 2D domain.
.. code-block:: shell-session
I range: (1, 1) > 8 , 8 ? 8,8< Enter >
J range: (1, 1) >2,40 ? 2,40< Enter >
Average or sum over J? (N) > ? < Enter >
K range: (1, 1) > ? < Enter >
Specify where to output the data. Press Enter to select the default ``*``, which will send
the data to the terminal. Alternatively, specify a file name to save the data in a data file.
.. code-block:: shell-session
File: (*) > ? <Enter> prints to screen
(filename<Enter> saves to filename)
X = 6.5000
Z = - 0.20000
Time = 0.10075
Y EP_g
1.0000 0.43971
3.0000 0.45994
....etc....
After the output is generated, you will be presented with a prompt to continue data extraction or analysis. Type
`q` and Enter to return to the main menu. From the main menu, type `0` and Enter
to exit .
.. code-block:: shell-session
Time: (1.000, 1.000) > q ? q< Enter > to quit
< main menu is displayed again >
Enter menu selection > 0 ? 0< Enter > to exit
.. include:: /icons.rst