Run

  1. Documentation
  2. Run

How to run the code to solve a real problem

To set up the run folder, for solving a problem, few input files are needed by the FEST-3D solver. To facilitate the process of setting up all these input files, a Python code is provided at Github.

Dependencies

  • C++11 compiler
  • Python 3
  • bash

Inputs

First, we need to create a directory to perform simulation and save all the input/output data.
RunDir = 'Test' Give any name to the Run directory

One of the important input is the grid/mesh files. FEST-3D code requires a separate file for each process. If the domain is decomposed into 4 blocks, then 4 separate files are required. Although, you can give any unique name to the grid files, for simplicity the python code expect grid file name in grid_nn.txt, where the nn is the block-number-1. So, for 4 blocks, we will use the following: grid_00.txt, grid_01.txt, grid_02.txt, and grid_03.txt. You should keep all the grid files in a separate folder and mention name of that folder at
GridDir='Mesh', here Mesh is the folder in which all the grid files are kept.
For more details about the grid/mesh read the subsection Mesh
NumberOfBlocks = 1 Total number of blocks
Now, you are required to fix different input parameter of the solver based on the problem you are simulating. Meaning of the most input is self-explanatory from the name.

Variable Expected Input Description
Control['CFL'] Real Number greater than zero Courant–Friedrichs–Lewy number. Low value (less than 1) for explicit scheme and high value for implicit scheme
Control['LoadLevel'] Integer Restart folder number in the time_directories/ directory
Control['MaxIterations'] Integer greater than SaveIterations Maximum number of iteration
Control['SaveIterations'] Integer lesser than MaxIterations Save solution state after every these many iteration
Control['OutputFileFormat'] 'vtk' or 'tecplot' Format of the solution output file
Control['OutputDataFormat'] 'ASCII' Type of the data in the output folder. Only ASCII for now. BINARY will be added in later release
Control['InputFileFormat'] 'vtk' or 'tecplot' Format of the solution file from which solution will be restarted
Control['InputDataFormat'] 'ASCII' Type of the data in the restart file
. Similar to output data type, only ASCII is supported for now.
Control['Precision'] Integer, lesser than 14 and greater than 1 Data precision for residual output, not used for solution output.
Control['Purge'] Integer Number of recent solution folder to keep and delete others. 0 input will keep all the folders
Control['ResidualWriteInterval'] Integer greater than zero Number of iteration after which to save the residual output in the file
Control['Tolerance'] Real number and ["Mass_abs", "Viscous_abs", "Mass_abs", "Resnorm_abs", "Viscous_abs", "Turbulent_abs", "Continuity_abs", "X-mom_abs", "Y-mom_abs", "Z-mom_abs", "Energy_abs", "Mass_rel", "Resnorm_rel", "Viscous_rel", "Turublent_rel", "Continuity_abs", "X-mom_rel", "Y-mom_rel", "Z-mom_rel", "Energy_rel", "TKE_abs", "Tv_abs", "Dissipation_abs", "Omega_abs", "Kl_abs", "TKE_rel", "Tv_rel", "Dissipation_rel", "Omega_rel", "Kl_rel"] Tolerance value and variable. The solver will stop once this value is achived. List of tolerace variables is given in expected input column. You can use only one input at a time.
Control['DebugLevel'] 1, 2, 3, 4, or 5 Print the information about the function/subroutines called in the solver. This helps in debugging the code. 5-Only important information is logged, 1-All the information is logged which helps in debuging. Will be remove in later release
Scheme['InviscidFlux'] 'ausm', 'slau', 'ausmUP', or 'ldfss0' Scheme to calcualte inviscid fluxes through cell faces
Scheme['FaceState'] 'none', 'muscl', 'ppm', or 'weno' Scheme for higher-order face-state reconstuction
Scheme['Limiter'] '1 1 1 0 0 0' or '0 0 0 0 0 0' Switch for limiters and pressure based switching when using higher order face-state reconstuction. Three value for i,j, and k direction 1->on and 0-> off. Koren limiter is being used with MUSCL scheme.
Scheme['TurbulenceLimiter'] '1 1 1' or '0 0 0' Switch for limiters when used for higher-order face-state reconstuctio of turbulent variables. 1->on and 0-> off
Scheme['TurbulenceModel'] 'none', 'sa', 'sst', or 'sst2003' Turbulence model
Scheme['TransitionModel'] 'none', 'bc', 'lctm2015' Transition model
Scheme['TimeStep'] 'l' or 'g [optional time step]' Time-step for time-integration. 'l' for local and 'g' for global. In case for global method you can provide exact value to time-step here.
Scheme['TimeIntegration'] 'none', 'RK2', 'RK4', 'TVDRK2', 'TVDRK3', 'implicit', or 'plusgs' Method for time-integration
Scheme['HigherOrderBC'] 0 or 1 Higher order boundary conditions. 1->on and 0-> off.
Flow["NumberOfVariables"] 5 Total number of variables to solver. Reduntant and will be depricated in later release.
Flow["DensityInf"] Real Number Free-stream density
Flow["UInf"] Real Number Free-stream x-component of velocity
Flow["VInf"] Real Number Free-stream y-component of velocity
Flow["WInf"] Real Number Free-stream z-component of velocity
Flow["PressureInf"] Real Number Free-stream pressure
Flow["TurbulenceIntensity"] Real Number Free-stream trubulent intensity in (percentage)
Flow["ViscosityRatio"] Real Number Free-stream ratio of turbulence viscosity to molecular viscosity
Flow["Intermitency"] Real Number Free-stream turbulent intermittency
Flow["ReferenceViscosity"] Real Number Reference viscosity
Flow["ViscosityLaw"] 'sutherland_law' or 'constant' Law used for viscosity variation
Flow["ReferenceTemp"] Real Number Reference temperature for viscosity variation
Flow["SutherlandTemp"] Real Number Sutherland temperature
Flow["PrandtlNumbers"] Two real numbers Prandtl number and turbulent prandtl number
Flow["SpecificHeatRatio"] Real number Specific heat ratio
Flow["GasConstant"] Real Gas Constant
OutputControl['Out'] [ "Velocity" , "Density" , "Pressure" , "Mu" , "Mu_t" , "TKE" , "Omega" , "kL" , "tv" , "Wall_distance" , "DuDx", "Dudy", "DuDz" , "DvDx", "DvDy", "DvDz" , "DwDx", "DWDy", "DwDz" , "DTDx", "DTDy", "DTDz" , "DtkDx", "DtkDy", "DtkDz" , "DtwDx", "DtwDy", "DtwDz" , "DtvDx", "DtvDy", "DtvDz" , "DtkLDx", "DtkLDy", "DtkLDz"] Variables to write in the output file
OutputControl['In'] ["Velocity" ,"Density" ,"Pressure" ,"viscosity" ,"TKE" ,"Omega" ,"kL" ,"tv"] Variables to read in case of restrart
ResidualControl['Out'] ["Mass_abs", "Viscous_abs", "Mass_abs", "Resnorm_abs", "Viscous_abs", "Turbulent_abs", "Continuity_abs", "X-mom_abs", "Y-mom_abs", "Z-mom_abs", "Energy_abs", "Mass_rel", "Resnorm_rel", "Viscous_rel", "Turublent_rel", "Continuity_abs", "X-mom_rel", "Y-mom_rel", "Z-mom_rel", "Energy_rel", "TKE_abs", "Tv_abs", "Dissipation_abs", "Omega_abs", "Kl_abs", "TKE_rel", "Tv_rel", "Dissipation_rel", "Omega_rel", "Kl_rel"] Residual to write in the resnorm file
BoundaryConditions [-3, -4, -5, -8, -6, -6] where <-1:'SUPERSONIC INLET', -2:'SUPERSONIC OUTFLOW', -3:'SUBSONIC INFLOW', -4:'SUBSONIC OUTFLOW', -5:'WALL', -6:'SYMMETRY', -7:'Pole', -8:'Far-field', -11:'Total inlet'> Boundary conditions to used for the six face of the domain 
$python edit-automaton.py

Directory structure

Executing edit-automaton.py will create a directory with usual directory structure:

  • system:all the input files including the mesh files and boundary condition file is located in this directory
  • time_directory: all the output files will be stored in this folder.
  • bin: a soft link between original FEST-3D binary is stored here.
  • run.sh: bash script to run the solver. This helps to remove log clutter on screen and save it in a log file named out in the time_directory/aux/ directory along with resnorm file which store the residual values.

Check Layout file

Although, edit-automaton.py python script tries to handle the boundary condition by its own; it is still not full-proof. So, always the check the layout.md file in the system/mesh/layout directory. Make sure all the boundary condition number are as you expect. In the case of pole boundary condition, some random number will be mentioned and required to change manually to -007. The layout file in explained in the later section.

Execute

$mpiexec.hydra -np 16 bin/FEST3D

On linux os you can use following command to run FEST-3D in the background:
nohup bash run.sh &

Check Status

The screen output is directed to the text file: [RunDir]/time_directories/aux/out
The residual are stored in the text file: [RunDir]/time_directories/aux/resnorm
You can output the current status or Current iteration number of the run on screen using

tail -f time_directories/aux/out

or you can check the residual by using Gnuplot or other similar software:

gnuplot gnplt

gnplt is the script provided for the Gnuplot software. You can download Gnuplot using:

sudo apt-get install gnuplot

Use ctl-c to stop the Gnuplot.

Post Processing

Since FEST-3D output solution file in Tecplot and VTK format, you can use either commerical TECPLOT software or open-source softwares like: Visit, Paraview, Mayavi.