Supersonic inviscid flow of Mach 2.0 past a 15-degree ramp

Contour of u speed — Fig.1 Mach contours simlulated with FEST-3D for supersonic flow over a 15-degree ramp.

Problem Statement

In this test case, a supersonic inviscid flow of Mach 2.0 past a 15-degree ramp will be simulated. The domain used, and boundary condition applied to the domain are illustrated in Fig. 2. The case definition and grid used were obtained from NPARC Alliance Validation Archive.

Mesh

A structured grid of size 153 × 91 × 2 will be used, as shown in Fig. 3. The grid is available in the tutorial folder |rootFolder|/run/Tutorial/Ramp/CreateBlocks/.

Note

If run folder is empty, please download the content from Github direcotry or download the zip file here.

In the blocking_point.f90 edit the number of blocks in the I-direction and J-direction. In this test case, only one block will be used.
integer, parameter :: xblocks = 1
integer, parameter :: yblocks = 1
In order to compile the blocking_point.f90 code with gfortran and execute it, commands are written in the makefile. Just use the following command to generate grid files in the grid/ folder.

$make

Run the previous command in the |rootFolder|/run/Tutorial/Ramp/CreateBlocks/ directory.

mesh — Fig.3 The Mesh for supersonic flow over a 15-degree ramp.

Setup

In order to setup the case directory, a python automation script is provided: automaton.py. First setup the most important parameters, the paths to the grid files and main executable binary to FEST-3D

RunDir = 'GiveAnyName' Name of the run directory to create for current case. You can give any name for this directory. This new directory will contains all the required files. All following command expect python automaton.py will be executed in this directory.

GridDir= 'CreateBlocks/grid/' Path to the folder which only contains grid file.
NumberOfBlocks = 1 Total number of blocks. It should match with number of gridfiles avaiable in the GridDir folder

AbsBinaryPath="/home/usr/FEST3D/bin/FEST3D"

Absolute path to the FEST-3D binary. Should be in |rootfolder|/bin/FEST3D
Now provide the common control parameters.
Control['CFL'] = 10.0 High CFL since implicit time-integration method will be used.
Control['LoadLevel'] = 0Since simulation will be started from scratch, 0 is specified.
Control['MaxIterations'] = 4000 Maximum number of iteration to perform.
Control['SaveIterations'] = 1000 Solution folder will be written every 1000 iteration.
Control['OutputFileFormat'] = 'tecplot' Type of solution file to write. If you have vtk file viewer you can user vtk instead of tecplot
Control['Purge'] = 1 Only one latest solution folder will be kept in the time_directories and rest will be deleted.
Control['ResidualWriteInterval'] = 5Write residual in time_directories/aux/resnorm after every 5 iteration.
Control['Tolerance'] = "1e-13 Continuity_abs" Stop the iteration if the absolute residual value of continuity equation is less than 1e-13.
Few scheme parameters for inviscid flow:
Scheme['InviscidFlux'] = 'slau' Inviscid flux-reconstruction shceme. You can use: ausm, ldfss0, ausmP , and ausmUP instead of __slau.
Scheme['FaceState'] = 'muscl' Higher-order face-state reconstruction method. you can use: none, ppm, and weno.
Scheme['Limiter'] = '1 1 1 0 0 0' Switch on the limiter for I,J,and K direction and switch of pressure based switching for all direction.
Scheme['TimeStep']='l' Local time-stepping method. You can use global time-stepping method also g.
Scheme['TimeIntegration']='implicit' LU-SGS matrix-free time integration method.
Now, lets define the flow feature of test case:
Flow["DensityInf"] = 1.225 Free-stream density.
Flow["UInf"] = 680.588 Free-stream x-component of velcotiy vector.
Flow["VInf"] = 0.0 Free-stream y-component of velcotiy vector.
Flow["WInf"] = 0.0 Free-stream z-component of velcotiy vector.
Flow["PressureInf"] = 101325.0 Free-stream pressure.
Flow["ReferenceViscosity"] = 0.0 Set reference viscosity to zero for inviscid flow.

OutputControl['Out'] = ["Velocity", "Density", "Pressure"] Variables to write in the output file.
ResidualControl['Out'] = ["Mass_abs", "Viscous_abs", "Continuity_abs"] Residual to write in the resnorm file.
BoundaryConditions = [-1, -2, -6, -6, -6, -6] Broad boundary condition.[supersonic inlet, supersonic outlet, rest are Slip-walls].

Rest of the variables should be left to thier default value. In order to execute this script use following command:

$python automaton.py

Now you will see a new folder created with RunDir name. Switch to that directory to run the test case. To make sure setup is correct, check the layout.md file located in system/mesh/layout/layout.md. The file should look like following:

## BLOCK LAYOUT FILE
## ==========================
## NUMBER OF PROCESSES
1
## NUMBER OF ENTRIES PER PROCESS
9
## PROCESS_NO GRID BC_FILE IMIN IMAX JMIN JMAX KMIN KMAX
## ===================================
## PROCESS 0
00  grid_00.txt  bc_00.md  -001  -002  -006  -006  -006  -006

The last line, in sequence, indicates the following:

Block_Number    GridFile   Boundary_condition_file   Imin_boundary_condition_number    Imax_boundary_condition_number Jmin_boundary_condition_number Jmax_boundary_condition_number Kmin_boundary_condition_number  Kmax_boundary_condition_number

Finally, to run the simulation use following command:

$nohup bash run.sh &

nohup helps in avoiding any output on the screen, & execute the last command in the background, allowing you to keep using the terminal.

Results

Contour of v speed — Fig.5 Surface pressure comparasion with theory.

Documentation

Supersonic flow over Wedge