• Using the Programs
  1. Example 1: One-Dimensional Shock Tube
  2. Example 2: Flow Over a Cone
  3. Example 3: Transient Flow over a Cylinder
  4. Example 4: Transient Flow over the Muses-C Capsule
  5. A Note on Dimensions
• Back to Contents Page

Using the Programs

The simulation proceeds in stages:

1. Prepare a script file that describes the flow problem and use scriptit to interpret this script and produce a Bezier Boundary File and an Input parameter File. Since these files are plain text files, they may be prepared "by hand" using any text editor. However, the script file approach is preferred.
2. Use the pre-processor mb_prep to read the flow description from the Input Parameter File and the Bezier Boundary File and then produce discretised descriptions of the flow geometry and the initial flow state. These are stored in a Grid File and an Initial Solution File respectively.
3. Use the main integration program mb_cns to read the discretised descriptions of the flow geometry and initial flow state, integrate the flow state forward in time and produce a new Solution File (which may contain the flow state at several times) and a History File (which may contain flow history data for a number of fixed points).
4. The postprocessing stage may involve the extraction of profile data using mb_prof or the reformatting of the flow solution data with mb_post. The data may be reformatted to a form that can then be imported to TECPLOT, MATLAB, EnSight, or the visualisation program mb_cont. The flow history for selected cells can be extracted with the postprocessor mb_hist.

Example 1: One-Dimensional Shock Tube

Move into the mb_cns/work/sod2 directory and copy the files sod2.p and sod2.bez from the mb_cns/examples/sod2 directory. The files sod2.p and sod2.bez contain the input parameters for the simulation and the Bezier geometry data as discussed above. They could be generated from the sod2.sit script by the scriptit program.

Assuming that your path includes the directory $HOME/cfd_bin, invoke the preprocessor with the command

% mb_prep.exe -f sod2

% mb_cns.exe -f sod2

The flow solution will be written to the file sod2.s and a history file sod2.h will also be written. The postprocessor mb_post.exe may be used to reformat the flow solution for plotting.

Alternatively, mb_prof.exe may be used to extract a profile of the flow solution (from sod.s) along one of the coordinate directions. The data for the plots in Report 10/96 were obtained by asking for two strips, one from block 0 and the other from block 1, but both with iy=1.

% mb_prof.exe -fp sod2.p -fg sod2.g -fs sod2.s -fo sod2.dat \
              -yline 0 1 -yline 1 1

Example 2: Flow over a Cone

This is a good example for exercising the codes when first installing them on a new machine. The simulation is short, on the order of a few seconds, and the output graphic is produced as a GIF file which can be viewed with a Web browser. If all goes well, you should see an image as shown below.

The simulation is of the transient flow following a shock as it travels over a 20 degree cone. The simulation is stopped after 300 steps, shortly after the shock has passed out of the right-most boundary. The flow should eventually settle to a conically-symmetric flow but, because the simulation has been stopped short, the bow shock propagating from the apex is clearly curved near the right boundary.

Move into the mb_cns/work/cone20 directory and copy the files cone20.sit and cone20.sh from the mb_cns/examples/cone20 directory.

The following figure, showing coloured pressure contours for the cone20 test case, was produced by running the shell script cone20.sh

#! /bin/sh
# cone20.sh
# exercise the Navier-Stokes solver for the Cone20 test case.
# It is assumed that the path is set correctly.

# Generate the Bezier and Input parameter files from the Script File.
scriptit.exe < cone20.sit > cone20.log

# Generate the Grid and Initial Solution Files.
mb_prep.exe -f cone20

# Integrate the solution in time.
mb_cns.exe -f cone20

# Extract the solution data and reformat.
mb_post.exe -fp cone20.p -fg cone20.g -fs cone20.s \
   -fo cone20 -generic

# Pick up the reformatted data and make a contour plot.
mb_cont.exe -fi cone20.gen -fo cone20.gif -var 6 -gif \
   -colour -mirror -xrange 0.0 1.0 0.5 -yrange -1.0 1.0 0.5

echo At this point, we should have a plotted solution in cone20.gif

CPU times for the 300-step version of this test case:

• 267 sec on a Toshiba Satellite T2130CS (i486 processor)
  (556 microsec per cell per p-c time-step)
• 102 sec on a Pentium-133 with the Watcom 10.6 compiler
  (212 microsec per cell per p-c time-step)
• 94 sec on a Pentium-133 with the EMX09c compiler
  (196 microsec per cell per p-c time-step)
• 66 sec on the same Pentium-133 running Linux
  (138 microsec per cell per p-c time-step)
• 69 sec on a 6x86MX-PR166 running Linux
  (144 microsec per cell per p-c time-step)
• 17 sec on a Pentium-II, 400MHz running Linux 5.1
  (35 microsec per cell per p-c time-step)
• 13.7 sec on a SUN Sparc Ultra-2
  (28.5 microsec per cell per p-c time-step)
• 9.5 sec on one (or maybe two) processor(s) of a Cray Origin 2000
  (19.8 microsec per cell per p-c time-step)

• 38.6 sec on a Celeron 2.0 GHz running Fedora Core 2, compiled with GNU C 3.3.2
  (21.8 microsec per cell per p-c time-step)

Example 3: Transient Flow over a Cylinder

The following figure, showing coloured density contours at an early time (5 microseconds) in the a98 simulation, was produced by running the shell script a98.bat on a Pentium based computer with MS-Windows-95.

Move into the mb_cns\work\a98 directory and copy the files a98.sit and a98_run.bat from the mb_cns\examples\a98 directory. The batch file to run the example contains the following text.

Rem  a98_run.bat
Rem  Exercise the Navier-Stokes solver for Amberyn's cylinder.

Rem  It is assumed that the path is set and that
Rem  the script file "a98.sit" has been correctly written.

Rem  Stage 1:
Rem  Generate the input parameter and Bezier files 
Rem  (a98.p and a98.bez respectively) from the script file.
Rem  A record of the transactions is recorded in the log file
Rem  "a98.log" so that, if anything goes wrong, you can browse
Rem  the log file and diagnose the problem.

scriptit < a98.sit > a98.log

Rem  Stage 2:
Rem  Pick up the input parameter and Bezier files
Rem  and generate the grid and initial solution files 
Rem  (a98.g and a98.s0).
Rem  Write these files as binary data.

mb_prep -wb -f a98

Rem  Stage 3:
Rem  Pick up the grid and initial solution files as
Rem  binary data and integrate the solution in time.
Rem  The solution data at later times will be written
Rem  to the solution output file "a98.s"

mb_cns -rb -wb -f a98

Rem  Stage 4:
Rem  At this point, we have a number of solution "frames"
Rem  in the solution output file "a98.s".
Rem  Extract the solution data at t = 5 microseconds 
Rem  and reformat so that the generic contour plotting
Rem  program can be used to generate an image.

mb_post -rb -fp a98.p -fg a98.g -fs a98.s -fo a98_05 -t 5.0e-6 -generic

Rem  Stage 5:
Rem  Pick up the reformatted data and make a contour plot.

mb_cont -fi a98_05.gen -fo a98_05.gif -gif -colour -mirror -xrange -0.005 0.015 0.005 -yrange -0.015 0.015 0.005

Rem  Finished:
Rem  At this point, we should have a density contour plot 
Rem  as a GIF image in in the file "a98_05.gif".
Rem  This GIF image can be viewed with any web browser.

CPU times for this test case:

• 4602 sec on a Pentium-133 with the Watcom 10.6 compiler
  (208 microsec per cell per p-c time-step)

The following animation, showing coloured density contours every 5 microseconds) in the a98 simulation, was produced by running the shell script a98_animate.bat to produce several GIF files which were then pasted together as an animated GIF image.

Further postprocessing can be done. For example, the following batch file produces a set of Tecplot data files, one for each time instant stored in the solution file, and then extracts the flow data along the stagnation streamline.

Rem  a98_post.bat
Rem  Further post-processing of the simulation of Amberyn's cylinder.

Rem  It is assumed that the solution files from the simulation
Rem  are in the current directory.

Rem  Pick up the solution data, extract the data for individual times
Rem  and generate a set of TECPLOT files

mb_post -rb -fp a98.p -fg a98.g -fs a98.s -t  5.0e-6 -fo a98_05 -tecplot
mb_post -rb -fp a98.p -fg a98.g -fs a98.s -t 10.0e-6 -fo a98_10 -tecplot
mb_post -rb -fp a98.p -fg a98.g -fs a98.s -t 15.0e-6 -fo a98_15 -tecplot
mb_post -rb -fp a98.p -fg a98.g -fs a98.s -t 20.0e-6 -fo a98_20 -tecplot
mb_post -rb -fp a98.p -fg a98.g -fs a98.s -t 25.0e-6 -fo a98_25 -tecplot
mb_post -rb -fp a98.p -fg a98.g -fs a98.s -t 30.0e-6 -fo a98_30 -tecplot
mb_post -rb -fp a98.p -fg a98.g -fs a98.s -t 35.0e-6 -fo a98_35 -tecplot
mb_post -rb -fp a98.p -fg a98.g -fs a98.s -t 40.0e-6 -fo a98_40 -tecplot

Rem  Pick up the solution and extract the data along the
Rem  stagnation steamline at t = 40 microseconds.
Rem  This line is close to the iy=1 line of cells in block 0.

mb_prof -rb -fp a98.p -fg a98.g -fs a98.s -t 40.0e-6 -fo a98_40.dat -yline 0 1

# a98_stag.gnu
# GNU Plot commands to produce a graph of temperature
# along the stagnation line.

set output "a98_stag.ps"
set terminal postscript eps

set title "Stagnation line Temperature"

set xlabel "x, metres"
set xrange [-0.005:0.0]
set xtics -0.004,0.002,0.0

set ylabel "T, degrees K"
set yrange [1500:4500]

plot "a98_40.dat" using 1:10

Example 4: Transient Flow over the Muses-C Capsule

The following figure shows coloured Mach number contours over a period of 80 microseconds for a Ben Stewart's Muses-C model in the X-2 expansion tube. The flow domain includes the last few centimetres of the expansion tube and part of the test section/dump tank. The gas is assumed to be inviscid, ideal air with a ratio of specific heats equal to 1.3. Note that the flow over the blunt nose of the capsule is established within 15 microseconds of shock arrival while the wake region is still developing slowly at the final time of 80 microseconds.

The simulation takes 4886 steps and requires the following CPU times:

• 4770 sec on a Pentium-133 running Linux
• 1189 sec on a Pentium-II/400 running Linux
• 1552 sec on (maybe) 4 processors of an Origin-2000; The wall-clock time was 404 seconds. To be fair, the grids for this case have few cells and there is a significant multi-tasking penalty associated with doing such a small (and poorly load-balanced) problem with 4 processors.

The script files can be found in the mb_cns/examples/cap directory.

• cap_run.sh sets up the parameter files and runs the simulation;
• cap_plot.sh extracts the solution frames and assembles the GIF animation;
• cap_mesh.sh can be used to generate a postscript plot of the mesh covering the flow domain;
• cap_prof.sh extracts the flow conditions around the blunt nose of the capsule at t = 80 microseconds and displays the pressure data using GNUplot.

A Note on Dimensions

An attempt has been made to adhere to ONE set of physical dimensions. Although the use of dimensional quantities within a CFD code is viewed as a weakness (and impure) by some CFD people, I made too many mistakes when converting between physical quantites and nondimensional parameters. The code therefore uses the SI-MKS unit system (i.e. metres, kilograms, seconds). However, the only place where units are encountered is in the gas.c module (where the physical properties of each gas are defined).