OS/2 Shareware BBS: 8 Other/08-Other.zip/ssiim14.zip/ssiim14.inf

OS/2 Help File | 1996-11-20 | 443KB | 3,697 lines

ΓòÉΓòÉΓòÉ 1. Introduction ΓòÉΓòÉΓòÉ


ΓòÉΓòÉΓòÉ 1.1. About this INF file. ΓòÉΓòÉΓòÉ

This file, ssiim.inf, is made from the SSIIM User's Manual. Most of the
equations are deleted, and some of the figures too. Some new figures are added,
especially in the examples


ΓòÉΓòÉΓòÉ 1.2. Foreword ΓòÉΓòÉΓòÉ

A THREE-DIMENSIONAL NUMERICAL MODEL FOR SIMULATION OF SEDIMENT MOVEMENTS IN
WATER INTAKES WITH MULTIBLOCK OPTION

Version 1.4

 The SSII model was developed in 1990-91 during the work with my dr. ing.
degree at the Division of Hydraulic Engineering at the Norwegian Institute of
Technology. SSII is an abbreviation for Sediment Simulation In Intakes. The
model was originally build around the numerical model Spider, which was made by
Prof. M. Melaaen during the work on his dr. ing. degree in 1989-90. Spider
solves a flow problem for a general three-dimensional geometry. SSII was made
up of sediment calculation routines for 3D solution of the convection-diffusion
equation for the sediments, communications with Spider and a graphical user
interface made in OS/2.

The main motivation for making SSII was the difficulty to simulate fine
sediments in physical models. The fine sediments, often under 0.2 mm, are
important for wear on turbines. It was also an advantage to be able to simulate
other problems as for example sediment filling of reservoirs and channels.

At the time SSII was made I had limited funding for computer equipment. This,
together with lack of knowledge of UNIX, made it necessary to develop the
models on a PC. Then a problem arouse, the 640 kB limit of DOS. The arrays that
the model used was often an order of magnitude larger than the DOS limit. The
DOS extenders were fairly unreliable at that time. Because of the long
computational times it was also important to have a multi- tasking operating
system. Therefore, the operating system OS/2 was used. Compared to UNIX, OS/2
is much more user-friendly, and this has been a major advantage during the
development process, giving increased productivity.

After finishing my dissertation in 1991, I wanted to improve the numerical
models. A disadvantage with the SSII and the Spider models for practical
situations was that a structured grid was used, and it was only possible to
have one block for an outblocked region. A natural improvement was a
multi-block model with general outblocking possibilities. This meant
considerable changes in Spider. Instead, a new water flow module for
multi-block calculation was made. This model was added to SSII, and the
resulting model was called SSIIM.

SSIIM, version 1.0, was uploaded on the Internet 17th of June 1993. Version 1.1
had some bug-corrections and some improvements in the water flow calculation
for multiple blocks. Version 1.1 was uploaded on the net 18th of October 1993.
In the fall of 1993 version 1.2 was made, with an improved user interface, some
additional tools and a revised manual. It was uploaded on the net 22nd of
December 1993. It was also distributed by diskette to selected water
institutions in January 1994. Version 1.3 included several bug-fixes, improved
sediment calculation and improved graphics. This was uploaded on the net 5th of
April 1994. It took a while until version 1.4 was uploaded on the net, mainly
due to the OpenGL additions. This meant that OS/2 version 4.0 had to be used.
Version 1.4 also includes transient calculations of water flow, free surface
and sediment transport, water quality, a 2D depth-averaged water flow module
and improved graphics.

Future plans for SSIIM includes a version with non-structured grid. It is very
likely that the graphics presentation modules will be improved. There are also
plans to include SSIIM in the River System Simulator (Internet:
www.sintef.no/nhl/rss/), a commercial product made by SINTEF Civil and
Environmental Engineering.

Several people have provided me with insight into the various problems I have
encountered in the development of this program. I have benefitted greatly from
the knowledge of Prof. Melaaen at Telemark Institute of Technology, in the
science of computational fluid dynamics. In the topics of hydraulics and
sedimentation engineering I have learned from Prof. Lysne at Division of
Hydraulic and Environmental Engineering at the Norwegian University of Science
and Technology, and from Prof. Julien, Prof, Gessler, Prof. Wohl and Prof.
Bienkjewicz at Colorado State University. Knut Alfredsen helped me with
software and hardware problems during the work with my dissertation, making the
SSII model. Vijaya K. Singh at IBM Canada has helped me with the C compiler.
Dave Zenz and Suzy Deffeyes at IBM Visual Systems has helped me with the OpenGL
graphics. I would also like to thank the following people for helping me test
the program: Morten Skoglund, Oscar Jimenez, Aslak LЫvoll, Lars Abrahamsen,
Siri Stokseth, J. Chandrashekhar, Knut Alfredsen, Hild Andreassen, Hilde Marie
Kjellesvig, Md. Mahbubur Rahman, Tuva Cathrine Daae, Anne Sintic, Atle Harby,
Amirul Islam Khan, Noor Quasim Khan, Chris Bowles, Catherine Wilson and
Per-Ludvig Bjerke. Also thanks to Richard Hibbert, David Seed, Richard May,
Luca Barone, Isabelle Lavedrine and Norbert Jamot at HR Wallingford Ltd, U.K.
for their work and evaluation reports on SSIIM.

Trondheim, 18. November 1996

Nils Reidar BЫe Olsen


ΓòÉΓòÉΓòÉ 1.3. Model purpose and structure ΓòÉΓòÉΓòÉ

SSIIM is an abbreviation for Sediment Simulation In Intakes with Multiblock
option. The program is made for use in
River/Environmental/Hydraulic/Sedimentation Engineering. The main motivation
for the program is to simulate the sediment movements in general river/channel
geometries. This has shown to be difficult to do in physical model studies for
fine sediments.

The program solves the Navier-Stokes equations with the k-epsilon model on a
three-dimensional almost general non-orthogonal grid. The grid is structured. A
control volume method is used for the discretization, together with the
power-law scheme or the second order upwind scheme. The SIMPLE method is used
for the pressure coupling. The solution is implicit, also over the boundary of
the different blocks. This gives the velocity field in the geometry. The
velocities are used when solving the convection-diffusion equations for
different sediment sizes. This gives trap efficiency and sediment deposition
pattern.

The model has a user interface with capabilities of presenting graphical plots
of velocity vectors and scaler variables. The plots show a two-dimensional view
of the three- dimensional grid, in plan view, a cross-section or a longitudinal
profile. It is also possible to view the geometry in three dimensions. The
OpenGL graphics library has been used to make graphics with color shading and
3D views. Additionally it is possible to simulate particle animation for
visualization purposes. See http: //www.sintef.no/nhl/vass/vassdrag.html for
examples of graphics presentation for various cases.

The model includes several utilities which makes it easier to give input data.
The most commonly used data can be given in dialog boxes. Several of the
modules in the program can be run simultaneously as separate threads. This
exploits the multi-tasking capabilities in OS/2. There is an interactive
graphical grid editor with elliptic and transfinite interpolation. Grid and
some of the input data can be changed during the calculation. This can be
useful for convergence purposes, and also when optimizing the geometry with
respect to the flow field.

 Advice for new users are given, who also are recommended to try the tutorial


ΓòÉΓòÉΓòÉ 1.4. Limitations of the program and known bugs ΓòÉΓòÉΓòÉ

SSIIM version 1.4 requires OpenGL graphics libraries to be installed with OS/2.
These are included in OS/2 version 4.0 and later.

Some of the most important limitations of the program are listed below.

      * The program neglects non-orthogonal diffusive terms.
      * The program neglects stress terms for elements that are not at the
      boundary.
      * The grid lines in the vertical direction have to be completely
      vertical.
      * Internal walls cannot be used within two cells from a multi-block
      connection.
      * Kinematic viscosity and density of the fluid is equivalent to water at
      20 degrees Centergrade. This is hard-coded and can not be changed.
      * Fully turbulent flow is assumed.
 Also note that some combinations of different options may not have been
 tested, and then there is a risk of a bug in the program. Not all algorithms
 are implemented for the multi-block options, since this option is redundant in
 a new version with unstructured grid. The animation graphics routine is not
 maintained as well as the other routines, which means that this routine has
 some bugs. The time-dependent flow in connection with free surface is also not
 to well tested. The contour map graphics routine also has a bug in connection
 with the boundary between blocks, and also sometimes some contour lines are
 missing.

 If you find any serious bugs that are not mentioned above, I would appreciate
 if you let me know. Please use the following addresses:

 E-mail:        [e-mail]

 Ordinary mail:

  Nils R. Olsen
  SINTEF Civil and Environmental Engineering
  Klaebuvn. 153
  7034 Trondheim
  Norway


ΓòÉΓòÉΓòÉ 1.5. Disclaimer and legal matters ΓòÉΓòÉΓòÉ

I disclaim all warranties with regard to this software and the information in
this document, whether expressed or implied, including without limitation,
warranties of fitness and merchantability. In no event shall I or my employer,
SINTEF, be liable for any special, indirect or consequential damages or any
damages whatsoever resulting from loss of use, data or profits, whether in an
action of contract, negligence or other tortuous action, arising out of or in
connection with the use or performance of this software. It is therefore not
recommended that the program be used for solving a problem whose incorrect
solution could lead to injury to a person or loss of property. If you do use
the program in such a manner, it is at your own risk. It is necessary to know
that to understand and interpret the program results properly it is required
that the user have knowledge and experience in computational fluid dynamics and
hydraulic engineering.

If results from SSIIM are used in a publication, this should be stated in the
publication.

Provided the user complies with the above statements, the program can be used
freely. The program can be distributed freely on condition that an unchanged
copy of this manual is distributed with the program.

Nils Reidar B. Olsen


ΓòÉΓòÉΓòÉ 2. Theoretical basis ΓòÉΓòÉΓòÉ

Some of the theoretical basis is explained in this chapter. For more details,
including the equations, see the written manual or some of the literature.


ΓòÉΓòÉΓòÉ 2.1. Standard water flow calculation ΓòÉΓòÉΓòÉ

The initial water surface is generated by a standard one-dimensional backwater
calculation. The friction loss is calculated by Manning's formula, using the
friction factor given on the W 1 data set in the control file. A separate
Manning's friction factor for each cross- section can be given on the W 5 data
set. This prescribed water surface can afterwards be changed according to the
calculated pressure field. The parameters for this procedure is given on the G
6 and the K 1  data set in the control file. It is also possible for the user
to specify the water surface. This is done by setting the  K 1 data set in the
control file to K 1 0 0, and adding the vertical level of each grid
intersection in the koordina file. In this way it is possible to simulate for
example a tunnel.

The Navier-Stokes equations for turbulent flow in a general three-dimensional
geometry are solved to obtain the water velocity. Alternatively, it is possible
to use a depth-averaged two-dimensional model. This can be specified on the F
44 data set of the control file. The k-Γûá model is used for calculating the
turbulent shear stress. A simpler turbulence model can be used for the
two-dimensional calculation. This is then specified on the F 43 data set of the
control file.

The equations are discretized with a control-volume approach. An implicit
solver is used,  also for the multi-block option. The SIMPLE method is the
default method used for  pressure-correction. The SIMPLEC method is invoked by
the K 9 data set in the control file.  The power-law scheme or the second-order
upwind scheme is used in the discretization  of the convective terms. This is
determined by the values on the K 6 data set in the control file. The numerical
methods are further described by Patankar (1980),  Melaaen (1992) and Olsen
(1991).

The default algorithm in SSIIM neglects the transient term. To include this in
the calculations the F 33 data set in the control file  is used. The time step
and number of inner iterations are given on this data set. For transient
calculations it is possible to give the water levels and discharges as input
time series. The timei file is then used.

The gravity term is not included in the standard algorithms. It is however
invoked in some of the free surface calculations.

Wall laws for rough boundaries are used. These are given by Schlichting (1979).
The roughness, ks, is equivalent to the diameter of particles on the bed. It
can be specified on the  F 16 data set in the  control file. If the roughness
varies at the bed, a roughness for each bed cell can be given in the  bedrough
file.

Influence of sediment concentration on the water flow

Note that there is still a discussion about the following arguments in the
science of sediment transport. Some of the explanations below are not generally
agreed upon.

The effect of the sediment concentration on the water flow can be divided in
two physical phenomena:

1. The sediment close to the bed move by jumping up into the flow and settling
again. This causes the water close to the bed to loose some of its velocity,
because some of the energy is used for moving the sediments. This can be
thought of as an added roughness. Einstein and Ning Chen [ 19] conducted a set
of classical experiments where they obtained a modified velocity distribution
as a function of the sediment concentration. This function modifies kappa in
the law wall. This formula is coded in SSIIM, and invoked automatically
whenever the sediment concentration array has values above zero, and the water
flow calculation is done.

2. The other phenomena is that the sediment concentration increase the density
of the fluid, which changes the flow characteristics. A typical example is a
density current. This effect is added as an extra term in the Navier-Stokes
equations. This term is not automatically invoked.  The user can invoke this
term by using the F 18 data set in the control file.

Note that the two effects will push the velocity profile in opposite
directions. Effect 1 will decrease the water velocity close to the bed, while
effect 2 will increase the water velocity close to the bed.


ΓòÉΓòÉΓòÉ 2.2. Sediment flow calculation ΓòÉΓòÉΓòÉ

 SSIIM calculates sediment transport by size fractions. In the control file,
each fraction is specified on an S data set, where the diameter and fall
velocity is given. This data set has to be given when calculating sediment
transport. The number of sediment sizes is given on the G 1 data set.

There are two ways to specify sediment inflow in the control file. One way is
to give the inflow on the I data sets in kg/s. An I data set must then be given
for each fraction. A vertical sediment concentration distribution will then be
used. This sediment concentration will be given over the entire upstream
cross-section (i=1).

The other way to specify sediment inflow is to use the G 5 data set. Then the
concentration is given for a specified surface at the boundary of the grid. The
concentration is given in volume fraction, which is used in all calculations by
SSIIM.

It is possible to use both I and G 5 options simultaneously to specify two
sources of sediments.

Sediment transport is traditionally divided in bedload and suspended load. The
suspended load can be calculated with the convection-diffusion equation for the
sediment concentration, c. In SSIIM the concentration is calculated by volume
fraction, and not by mass fraction.  The fall velocity of the sediment
particles is denoted w. The diffusion coefficient is taken from the k-epsilon
model. The Schmidt number is set to 1.0 as default. If the user want a
different number, this can be set on the F 12 data set in the control file.

The concentration in the elements closest to the bed can be found by various
methods described below. The concentration is "forced" on the bed boundary
finite volumes in a similar manner as the boundary condition for epsilon in the
k-epsilon model. The convection-diffusion equation is not solved for the cells
closest to the bed. Sediment continuity for these cells are therefore usually
not satisfied. The discrepancy in continuity is used to calculate changes in
the bed levels. This method also has the advantage of simulating the
interaction between the sediment that moves close to the bed and the sediment
that move in suspension.

Van Rijn (1987) developed a formula for the equilibrium sediment concentration
close to the bed.

Another approach is to use a formula for total load, for example
Engelund/Hansen's (1967) formula, together with the theoretical vertical
sediment and water velocity distribution for uniform flow.

In SSIIM version 1.2 there were many different options for determining the bed
concentration. Since then a block-correction method has been added to the
sediment concentration solver. This meant a major improvement in convergence,
and also the difference between the various methods became smaller. The choice
of initial bed grain size distribution and recalculation algorithm is given on
the F 30 data set.

It is possible to calculate transient sediment transport. A transient term is
included in the differential equation. This algorithm is invoked on the F 36
data set.

For the calculation of bed grain size distribution, this algorithm divides the
bed in two layers: an upper layer at the bed surface, and the one below. The
bed grain size distribution is recalculated based on a budget method for the
upper layer. The thickness of the surface layer is set equal to the largest
grain size. To avoid unphysical results, the upper layer is not allowed to
erode a vertical distance more than the thickness of the upper layer during one
time step. This applies only if multiple grain sizes are used. This limitation
has the effect that too low erosion rates can be observed if the maximum grain
size is small and the time steps are long.


ΓòÉΓòÉΓòÉ 2.3. Porosity calculation ΓòÉΓòÉΓòÉ

A roughness element in a complex geometry can always be modeled by providing
fine enough grid to dissolve the boundary of the roughness element. The
disadvantage with this method is that the number of grid cells may be too
excessive for practical use. Instead, the roughness elements can be modeled
within each grid cell. This can be done in two ways, depending on the magnitude
of the roughness elements. If the magnitude is fairly small compared to the
size of the grid cell, the roughness can be incorporated in the law of the
wall. If the roughness elements are larger, other methods must be used. The
porosity model used in SSIIM is developed by Engelund (1953):

Note that the porosity will also affect the turbulence in the flow field. To
model this it would be necessary to modify the k-epsilon turbulence model. This
is not done in this study. It is assumed that the source term given by the
porosity model is so great that it dominates over the turbulent diffusive
terms. Then the values of k and epsilon in the porous domain will only have
negligible effects on the flow field.

The porous domain is defined by the user for each cell as a distance above the
bed. The grid lines in the vertical direction is completely vertical and
parallel. This means that for each horizontal projection of the grid, one must
search for the cell where the top of the porosity is located. Wall functions
are applied in this cell, and the porosity model is applied for the cells
below. In the porous area the values for k are set to 0.01, and the values for
epsilon are set according to wall laws.

The porosity is calculated using a routine which is based on a set of measured
depths at different locations in the river. For each significant rock in the
river points are taken on top of the rock and on its sides. Thus, several
points are taken for each bed element. The porosity generation model finds all
the points in each bed cell, and calculates how many points are located within
certain elevations. The top elevation is taken to be equal to the elevation of
the highest point in the cell.

The porosity, pmin, at the bed level is given as a user input.

For each cell the porosity is calculated from interpolation from the set of
porosities as a function of the elevation.

The porosity calculation is further described by Olsen and Stokseth (1995).

Calculations with porosity have to use a P on the F 7 data set in the control
file, and the porosity data must be given in the porosity file.


ΓòÉΓòÉΓòÉ 2.4. Free surface calculation ΓòÉΓòÉΓòÉ

First, note that if a tunnel is simulated, and the user want to specify the
upper boundary, the K 1 data set in the control file should have the parameter
0, and the koordina file should be arranged accordingly.

There are several methods of calculating free surface in SSIIM. The standard
(default) method is to use a one-dimensional backwater calculation and use the
result as a fixed lid with zero gradients. Different Manning's friction factors
can be given for the various cross-sections on data set W 5 in the control
file, thereby allowing the user to make the appropriate lid.

The next alternative is to update the lid as a function of the calculated
pressure field. This is done on the G 6 data set in the control file. The user
gives which point in the grid that will not move, and the rest of the surface
grid moves according to the pressure field. This routine gives satisfactory
results for the curved channel example

There are two more alternatives, both coupled with the transient calculation.
The F 36 data set in the control file invokes the transient free calculation.
If the index is 2, than a routine similar to the routine of the G 6 data set is
used. This method is called method 2. The method does not necessary give the
correct flow field for a wave or a rapidly moving surface. If the surface has
only small movements, this method can be used. Note that this method does not
preserve water continuity.

If the index on the G 6 data set is 1, then another method is invoked.  This
method adds a gravity term in the Navier-Stokes equations. Thereby the
hydrostatic pressure field will result if the flow is uniform. The movement of
the water surface is based on the continuity defect in the cells closest to the
water surface. This is done instead of using the SIMPLE algorithm for these
cells. The method gives a more correct simulation of rapidly moving water
surfaces, as for example a flood wave. Water continuity is satisfied, contrary
to the other water surface calculation methods. The disadvantage is that the
calculation becomes more unstable. This is further discussed here


ΓòÉΓòÉΓòÉ 2.5. Water quality and temperature ΓòÉΓòÉΓòÉ

The water quality and temperature is calculated with the convection-diffusion
equation for the concentration of each variable, similar to the sediment
concentration. The difference is the addition of extra source and sink terms,
due to fluxes at the water surface and chemical and biological reactions. The
source (sink=negative source) terms in the equations have been modeled in a
number of different ways by various researchers and computer programs. It was
the goal of the implementation of water quality in SSIIM to give the user a
flexibility on how to model each term. The user must therefore not only specify
various reaction constants, but also specify each term in the source equation.
This is sligtly more laboreous than other models when making the input files,
but it gives better flexibility for the user to make new terms and models for
the various situations.

The user first have to decide how many constituents are to be simulated. Note
that the temperature is here defined as a water quality constituent. The user
have to number each variable from 0 to as many variables as is used. Presently,
the maximum number  of variables are 20. The number of variables have to be
given on the F 50 data set. The names of each variable is given in the control
file on the Q 0 data set. Note that only lowercase letters can be used, and a
maximum of 40 charachters. For each equation, the user have to specify the
source terms in the equations. This is done on the Q data set in the control
file. There are a number of various Q data sets, from Q 1, Q 2 ... etc. Each
data set gives a number of integers and floats. The first integer is always the
index for the equation.

Each term in each equation have its own Q data set. For example, if
temperature, oxygen and nitrogen is simulated, this gives three variables. The
following Q 0 data sets can then be used:

Q 0 0 temperature
Q 0 1 oxygen
Q 0 2 nitrogen

The source terms then have to be specified. For simplicity, let us say that the
temperature source is 0.1 times the oxygen concentration and the oxygen source
is 0.3 times the temperature. The nitrogen source is 2.1 times the oxygen
concentration multiplied with the temperature minus 0.4 times the nitrogen
concentration. This is then given as:

Q 1002 0 1.0 18.0
Q 1 2 1 0.3
Q 2 3 1 2 2.1
Q 1 3 2 -0.4

More details on the Q data sets are given here. Also, consult one of the
examples.

No more than 40 variables can be simulated, and it is not allowed to have more
than 200 Q data sets in the control file.

The above example shows the flexibility of the program to incorporate new
models for the various reactions. It also shows that the user is able to make
models that make little sense from a biological/chemical point of view, and the
program will allow this calulation to be carried out. The user must therefore
have a good knowledge of water quality processes to give reasonable input data
and to obtain reasonable results. Care must also be taken not to mis-type
numbers on the Q data sets.

In addition to this, the user must specify the inflow of each variable. This is
done on the G 18 data set. The concentration/temperature is specified together
with the geometrical location of the inflow and the time the inflow starts. No
more than 100 G 18 data sets can be used in the control file. Note that the G
18 data set has a parameter for when the inflow starts. This can be used to
specify a time series of inflow of a given variable.


ΓòÉΓòÉΓòÉ 3. User interface ΓòÉΓòÉΓòÉ

The main user interface appears once the program is started and the input files
are read or generated.

If a control file is not present, the user is prompted for the necessary
parameters in a dialog box. A default control file is then made and written to
the disk.

If a koordina file is not present a rectangular channel is made initially. A
dialog box appears, which prompts the user for the length and the width of the
channel. The bed levels of the channel will be at elevation 0.0. The water
depth is given in the dialog box for the control file, or on the W 1 data set
in the control file.

The main user interface consists of a dialog box and a menu bar. The dialog box
appears in the lower left corner of the screen, and the menu bar appears on the
middle left side of the screen. The dialog box does not have any editfields,
only text fields and a push button. The dialog box shows intermediate results.
The two top lines in the dialog box are text which is written from the
different modules. There are also six numbers on an exponential format. These
are the residuals for the six equations in the water flow calculation. The
push-button is used for refreshing the text and values in the dialog box.

The menu bar of the main user interface is used for starting different
sub-modules and showing graphics. The File option gives the possibility of
reading and writing different files. The Input Edit option gives the
possibility of editing the input data through a grid editor or dialog boxes.
The Computations option is used for starting the water flow or the sediment
calculations. The Graphics option is used for displaying the results in
different graphics windows.


ΓòÉΓòÉΓòÉ 3.1. Interactive input of parameters ΓòÉΓòÉΓòÉ

Some of the most commonly used parameters can be set in dialog boxes. These
dialog boxes are activated by the Input Edit choice in the main menu bar. The
choices are:

* Grid Editor

* Sediment data: This gives the grain size, fall velocity and inflow of each
grain size. Note that the number of grain sizes can not be changed.

* Sediment parameters: This gives various parameters for calculation of
sediment flow.

* Waterflow parameters: This gives various parameters for calculation of water
flow. This is an important dialog box that is used when there are convergence
problems and when parameter tests are done. Note that the parameters can be
changed while the program is calculating the water flow field.

Note that the parameters that can not be given in the dialog boxes have to be
given in the control file.


ΓòÉΓòÉΓòÉ 3.2. The Grid Editor ΓòÉΓòÉΓòÉ

 The grid editor is invoked by choosing GridEditor on the Input Edit choice in
the main menu. The user can click with the mouse on a grid intersection and
drag this to a new location. The mouse button must be pushed down while the
movement is made.

The main menu of the grid editor is made up of five main choices plus the Help
choice.

Move/Scale
Utility
Define
Generate

Note that after having edited the grid, it is advisable to write the content to
a koordina file. This is done in the File option of the main menu. A file named
koordina.new will be written. The attraction parameters and the fixed point
parameters can be written to the control.new file from the same sub-menu.


ΓòÉΓòÉΓòÉ 3.2.1. Move/Scale ΓòÉΓòÉΓòÉ

 The option Move is used to move the plot upwards, downwards or sideways. The
arrow keys can be used instead of the menu. The option Scale is used to
enlarge, shrink or distort the plot. The keys <Page Up> and <Page Down> can be
used for scaling. The option 2 Point Enlarge is used for enlarging a certain
section of the grid. After this choice is made, the user clicks at the lower
left corner and upper right corner of the part of the grid that the user wants
to see. After the second click the enlargement is made.


ΓòÉΓòÉΓòÉ 3.2.2. Utility ΓòÉΓòÉΓòÉ

 The option Utility has five choices on the pull-down menu. The first choice,
Show geometrical points, displays the points in the geodata file on the grid
plot. The points are shown with a square, and the different color indicate
different vertical levels.

 The second choice, Make bed interpolations, generates z values for the bed
surface of the grid. This is the same level as given in the koordina file. This
option can then be used to make the z values in the koordina file, if the
choice write koordina.new is made from the File option in the menu of the main
user interface. The bed interpolations are done in a separate thread in OS/2,
because the calculations may take some time. This allows other tasks to be
carried out during the interpolation.

 The z values are interpolated from a set of geometrical data read from the
geodata file. If there is no geodata file present, an error message is given.
The interpolation routine goes through all the grid points i,j, and finds the
closest points in the geodata file in all four quadrants where the grid
intersection (i,j) is the center of the coordinate system. Then a linear
interpolation from these four points is made. If one of the points in the
geodata file is closer than 5 cm from the grid point, this z value is chosen
and no interpolation is done. The outcome of the interpolation is logged to the
file boogie.bed. If the interpolation routine is unsuccessful in finding the
point, the z value is set to zero.

 The third choice, Apply changes, sets a global change flag. When the waterflow
routine sees that this flag is set it updates the calculation geometry
according to the grid editor geometry.

 The fourth choice, Read koordina.mod, reads x,y and z values for one or more
points in the grid. The data in the koordina.mod file is on the same format as
in the ordinary koordina file, but it is not required that all of the
coordinates are present in this file. This option is useful if a predefined
shape is wanted, for example a circle. Then the grid line intersections for the
circle can be generated with a spreadsheet, and only the points on the circle
is placed in the koordina.mod file. When this is read, the grid is moved
according to the points on the circle.

The fifth choice, New water level and grid, is used after having changed the z
values on any of the coordinates. The grid editor only moves the grid in the
layer bordering the bed. So if any of the grid points have been moved in the
vertical direction, the water level and the grid points above the bed needs to
be recalculated. This is done by using this option. Note that this will modify
the koordina file according to the changes that are made.


ΓòÉΓòÉΓòÉ 3.2.3. Define ΓòÉΓòÉΓòÉ

This option is used for defining different parameters. The parameters are often
connected to grid intersection points. The point that was last activated by the
mouse is used as default.

The first option is Give coordinates. This gives a dialog box where the user
can give numerical values for x,y and z for a grid intersection.

The second option is Set NoMovePoint. This invokes a mode where the user can
define certain points which will not be moved by the interpolation, called
NoMovePoints. In NoMovePoint mode it is not possible to move the grid points
with the mouse. When the user clicks on a grid intersection, a blue star
emerges on the intersection as a sign that this is chosen. Up to 200
NoMovePoints can be chosen. To verify that this mode is present, the letters
"Point mode, 0" is shown on the lower part of the editwindow when the Set
NoMovePoint is chosen. The integer shows how many points you have chosen. To
return to the normal mode, choose Define and Set NoMovePoint again. It is
verified that the normal mode is set because the text "Point mode" disappears.
In the normal mode the user can move all points including the NoMovePoints.

The third option is Delete NoMovePoint. This deletes the last point set under
the NoMovePoint mode.

 The following four options are setting of attraction to certain points or
lines in the grid. This is used by the elliptic grid generator. A dialog box
emerges when the choice is made, and the user must give two integers which
describes the location of the attraction point/line. Then two attraction
parameters are given. The Prop. att. value is proportional to the attraction.
If negative, the grid lines are moved away instead of attracted. The Sq. att.
value gives an attraction proportional to the grid line difference raised to a
power of Sq. att.. This value is used to determine how far out in the grid the
attraction works. Note that a smaller value will give larger attractions. If
the value of Prop. att. is negative, the grid lines are moved away instead of
attracted. Point attraction gives attraction to points, and Line attraction
gives attraction to lines. Up to 200 attraction points can be defined. The
attraction points can be seen on the grid by colored rectangles at the grid
intersections.

 The last option in the Define menu is Delete last attraction. This deletes the
last defined attraction.


ΓòÉΓòÉΓòÉ 3.2.4. Generate ΓòÉΓòÉΓòÉ

 The first choice in the pull-down menu is Boundary. This choice interpolates
linearly along the four border lines of the grid. Note that the z values are
also interpolated. This will create a rectangle unless a NoMovePoint has been
defined on the border. Then the interpolation will be between the corners and
the NoMovePoints.

 The second choice is Elliptic. This starts the elliptic grid generator. Note
that this will not change the z values.

 The third choice is TransfiniteI. This is transfinite interpolation in the
streamwise direction. The z values will be interpolated. In this mode the
NoMovePoints will also be moved.

The fourth choice is TransfiniteJ. This is the same as TransfiniteI, except it
is in the cross- streamwise direction.

The fifth choice is TransfiniteM. This is an average of TransfiniteI and
TransfiniteJ.

The sixth choice is Average. This is a procedure where the x,y and z values of
a grid intersection are taken to be the average of the four neighboring grid
intersections. This procedure is repeated for all the inner grid intersections.
This will not move the NoMovePoints.

Important notes:

1.   After having edited the grid, it is advisable to write the content to a
koordina file. This is done in the File option of the main menu. A file named
koordina.new will be written. The attraction parameters and the fixed point
parameters can be written to the control.new file from the same sub-menu.

2.   Using unfavorable attraction coefficients can cause the elliptic generator
to crash, which means that SSIIM also crashes, and the grid data are lost. It
is therefore adviceable to write the grid to files before starting the elliptic
generation with attraction coefficients.


ΓòÉΓòÉΓòÉ 3.3. Presentation graphics routines ΓòÉΓòÉΓòÉ

 There are ten graphics modules for presentation of results. These can be
invoked any time during the calculation or afterwards. More than one module can
run simultaneously. The modules are choices under the Graphics option of the
main menu:

The modules use the standard GUI for OS/2, and have approximately the same
system of menus.


ΓòÉΓòÉΓòÉ 3.3.1. OpenGL 2D ΓòÉΓòÉΓòÉ

OpenGL 2D will show a two-dimensional projection of a profile in the x,y or z
plane. The profile will follow a grid surface. A cross-section will be shown as
a projection in the yz plane, a longitudinal profile will be shown as a
projection in the xz plane and a plan will be shown as a projection in the xy
plane. Also, the velocity vectors may not be parallel to the grid. The x, y or
z components is used.

The variables will be displayed with color shading. The colors will always
display red as the maximum value, then yellow, then green and blue as the
minimum value. The user can choose from a number of variables.

Examples of OpenGL plots are given in: Flow in a curved channel Map of velocity
field in a reservoir


ΓòÉΓòÉΓòÉ 3.3.2. OpenGL 3D ΓòÉΓòÉΓòÉ

OpenGL 3D shows an orthographic projection of grid surfaces. If no surfaces are
specified on the G 19 data set in the control file, the bed of the geometry
will be shown. Several G 19 data sets can be used to specify three-dimensional
surfaces of the geometry. The figure can be rotated, scaled and moved. Various
options for variables can be displayed.


ΓòÉΓòÉΓòÉ 3.3.3. Map ΓòÉΓòÉΓòÉ

Map presents the geometry seen from above. It is possible to get velocity
vector plots and plots and bar plots of concentration, diffusivity, k, etc. It
is also possible to plot the grid and change between different vertical levels.


ΓòÉΓòÉΓòÉ 3.3.4. Contour map ΓòÉΓòÉΓòÉ

Contour map presents the variables as contour plots, seen from above. The user
can give the values of the contour lines on the L data set in the control file.
If the L data set is not given, seven contour lines will be used. These are
calculated to be within the range of the calculated variable field. If the
option Variable under Scale is chosen, the user can give the numerical values
of the lines. It is also possible to choose the number of lines. Note that if
more than 7 lines are chosen, all lines will be black. Also note that if 0
lines are chosen in the dialog box, the plotting will be similar to giving no L
data set in the control file.


ΓòÉΓòÉΓòÉ 3.3.5. Color map ΓòÉΓòÉΓòÉ

Color map presents the variables with colors and density patterns for each cell
depending on the value in the cell. This is seen from above. The user can give
different colors and shading pattern on the H data sets.


ΓòÉΓòÉΓòÉ 3.3.6. Longitudinal profile ΓòÉΓòÉΓòÉ

Longitudinal profile presents a longitudinal profile of the geometry. Graphs
with different parameters as a function of depth along the longitudinal profile
is obtained. It is also possible to view the grid or the velocity vectors. It
is possible to change between different longitudinal profiles.


ΓòÉΓòÉΓòÉ 3.3.7. Cross-section ΓòÉΓòÉΓòÉ

Cross-section presents a cross-section of the profile. It is only possible to
see a velocity vector profile. It is possible to change between different
cross-sections.


ΓòÉΓòÉΓòÉ 3.3.8. VerifyProfile ΓòÉΓòÉΓòÉ

VerifyProfile presents calculated profiles of concentration or velocity at
locations specified by the user. It also presents user-given data in the same
plot. Arrange the measured values in the verify file.


ΓòÉΓòÉΓòÉ 3.3.9. VerifyMap ΓòÉΓòÉΓòÉ

VerifyMap presents calculated and measured velocity vectors in the same figure.
Different colors and legends are used to differentiate the calculated and
measured vectors. Arrange the measured values in the verify file.


ΓòÉΓòÉΓòÉ 3.3.10. Animation ΓòÉΓòÉΓòÉ

 The purpose of the animation module is flow visualization. The module displays
the grid as seen from above, and animates the movement of a sediment particle.
The movement of the particle will depend on the flow field and the fall
velocity of the particle.

When the animation window starts, it checks a mouse scaling parameter. If this
is not provided in the G 15 data set in the control file, an X is written in
the window, and the user should click on this to make the program scale the
location of the mouse. If the user writes the control.new file from the main
menu, the correct G 15 data set is given in this file.

The animation window has five menu options. These are Move and Scale which are
similar to the other presentation windows. Then there is the Particle option.
The pull- down menu is used to set the particle size, which will be used by the
program to calculate a fall velocity. The next menu option is Run, which starts
the particle movement.

The particle starts from one point in the grid and always from the top cell in
the vertical direction. Then it moves along the geometry until it reaches one
of the cells that borders the boundary. Then it returns to the starting point.
The starting point is changed by clicking with the mouse at a location in the
geometry.

The last option in the animation window menu is Speed. By choosing Double or
Half the time step is doubled or divided by two. This choice can be repeated
for further increase or decrease in time step. Note however that if the time
step becomes large, the particle may not move along the steam lines any more,
and it may even move out of the geometry during the time step. The accuracy of
the particle trajectory will increase with decreasing time step.


ΓòÉΓòÉΓòÉ 3.4. Presentation graphics menu system ΓòÉΓòÉΓòÉ


ΓòÉΓòÉΓòÉ 3.4.1. Legend ΓòÉΓòÉΓòÉ

The OpenGL graphics has an option Legend. This shows the color legend of the
plot. It can be used in presentations by using a screen-capturing tool to move
one of the legends to the word processor. The maximum and minimum values are
shown in the bar above the menu.


ΓòÉΓòÉΓòÉ 3.4.2. Direction ΓòÉΓòÉΓòÉ

The OpenGL 2D graphics has an option Direction. This gives the choice of
displaying a cross-section, longitudinal profile or a plan view.


ΓòÉΓòÉΓòÉ 3.4.3. Rotate ΓòÉΓòÉΓòÉ

The OpenGL 3D graphics has an option Rotate. This gives the choice of rotating
the three-dimensional view around the x,y or z axis. Instead of using the menu,
it is possible to use the <F3> and <F4> keys to rotate around the x-axis, the
<F5> and <F6> keys to rotate around the y-axis and the <F11> and <F12> keys to
rotate around the z-axis.


ΓòÉΓòÉΓòÉ 3.4.4. Move ΓòÉΓòÉΓòÉ

The option Move is used to move the plot upwards, downwards or sideways. The
arrow keys can be used instead of the menu.


ΓòÉΓòÉΓòÉ 3.4.5. Scale ΓòÉΓòÉΓòÉ

The option Scale is used to enlarge, shrink or distort the plot. The keys <Page
Up> and <Page Down> can be used for scaling. Some of the graphs also use <CTL>
+ arrows for distorting the plot. The option 2 Point Enlarge is used for
enlarging a certain section of the grid. After this choice is made, the user
clicks at the lower left corner and upper right corner of the part of the grid
that the user wants to see. After the second click the enlargement is made.

For the OpenGL plots, sub-menu under Scale can be used to move the color scale
to red or blue. This is also visualized in the Legend view. The <F7> and <F8>
keys can be used for the same purpose. For the OpenGL 2D plots, the velocity
vectors can be turned on/off and enlarged/shrinked. The <F5> and <F6> keys
enlarges/shrinks the velocity vectors.


ΓòÉΓòÉΓòÉ 3.4.6. Graph ΓòÉΓòÉΓòÉ

The third option in the menu bar is Graph. The sub-menu displays different
parameters that can be shown. The option Sediment sample no. is a reference to
which of the N datasets from the control file is placed at which location at
the grid. The sub-menu option Bedchanges shows the bed changes during and after
sediment calculation. The sub-option Dominant grain size shows which bed grain
size has the highest fraction in each bed element. The ColorMap option is be
used for displaying a color map of some of the following parameters: water
depth, bed shear stress, turbulence, velocity and sediment size. The colors are
given by the user in the H data sets in the control file.

The sub-option L-val concentration is used to change between different grain
sizes. When choosing Sum, the sum of the different grain sizes (total
concentration) is shown. The three last options are used for changing which
two-dimensional slice is presented. The two first sub-sub options are i++, i--,
j++, j--, k++, k--, depending on which direction is changed. These options
chooses the next(++) or previous(--) slice.


ΓòÉΓòÉΓòÉ 3.4.7. Timer ΓòÉΓòÉΓòÉ

The next option on the menu bar is Timer. The timer is a module which updates
the graphics at certain time intervals. The numbers of the different
sub-options under Timer indicates the interval in seconds. The options Start
and End starts and stops the timer.


ΓòÉΓòÉΓòÉ 3.4.8. Copy to clipboard ΓòÉΓòÉΓòÉ

From the clipboard, the plot can be pasted directly into for example a word
processor that support the clipboard.

Also see Hardcopies


ΓòÉΓòÉΓòÉ 3.4.9. System/save ΓòÉΓòÉΓòÉ

The last option on the menu bar is System or Save. The pull-down menu of System
has the option Save. This is used for storing the plot in an OS/2 metafile. It
can then be printed or plotted on paper by the Picture Viewer utility that
comes with OS/2. The names of the metafiles file will be mapfl000.met,
longf000.met, color000.met, conto000.met, vprof000.met, bedfl000.met or
cross000.met, depending on which of the graphics procedures that produced the
file. If there is an existing file with the same name, this will not be
overwritten. Instead a new file with last charachters 001 instead of 000 will
be written. If this exist, further increments in the number in the name will be
made, until number 999.

Also see Hardcopies


ΓòÉΓòÉΓòÉ 3.4.10. Bedchange ΓòÉΓòÉΓòÉ

The other options from System is Bedchange+ and Bedchange-. These options only
have effects in the Map graphics. The option Bedchange+ activates the change in
the bed levels according to the calculated bed changes. Bedchange- changes the
bedlevels back. It is not recommended to use these, but instead use the
time-dependent calculations that are introduced in version 1.4.


ΓòÉΓòÉΓòÉ 3.5. Hardcopies ΓòÉΓòÉΓòÉ

 It is not possible to plot directly from SSIIM to a plotter. One must first
make a graphics file, or copy to the clipboard, and then use a word processor
or a drawing program to plot to the plotter. Slightly different techniques are
used to make copies from the OpenGL plots and the other plots.

Using the OpenGL graphics, it is necessary to use a screen capture utility to
make a copy to the clipboard or to make a bitmap file. This can for example be
done with the PmCamera utility, which is made by IBM. The program is freeware
and can be downloaded from internet sites. Start the program in a separate
window. PmCamera then gives a dialog box. Check on the "active window"
radiobutton, and on the "OS/2 Clipboard" checkbox. Then minimize the dialog box
with a click on the upper right icon. The program will then run in the
background and capture the graphics in the active window. Next, run SSIIM, and
display the OpenGL plot as you would like to have the hard-copy. Then push the
"PrintScreen" button on the keyboard, and wait until you have heard two beeps.
PmCamera has then copied the graphics to the clipboard. It is also possible to
let the PmCamera utility make a bitmap file, which can be stored.

To plot the OpenGL graphics from the clipboard, one can for example use the
IBMWORKS wordprocessor from the Bonus-pack. Start the word-processor, and
choose "paste" from the "edit" of the menu to copy from the clipboard. Then
print the result.

It is also possible to generate .gif files from the .bmp files using a freeware
tool bmpgif2.exe. This can be found on most os/2 Internet software sites. The
.gif files can be used in other types of presentation and word processing
software.

Using non-OpenGL graphics, it is possible to copy directly to the clipboard or
to a metafile from SSIIM. It is then also possible to use a word processor to
copy from the clipboard, or import the metafile and then print the results. A
useful utility which is bundeled with OS/2 is PicView, which plots the vector
graphics from the clipboard or from a metafile to the plotter.

Some advice when plotting on a pen plotter: If the lines of the plot are not
clear, leave the paper in the plotter and plot several times on the same paper.
This technique can also be used to get both vector and color plots on the same
figure.


ΓòÉΓòÉΓòÉ 4. Input/result files ΓòÉΓòÉΓòÉ

 most of the files are only used for special purposes and they are normally not
required. Some of the files are output files. The program can produces many of
the input files. For simpler cases all the necessary input files can be
generated by the program. The two main input files are the control file and the
koordina file. All the files are ASCII files, and can be created using a
standard editor.  SSIIM file structure for main files


ΓòÉΓòÉΓòÉ 4.1. The control file ΓòÉΓòÉΓòÉ

 The control file gives most of the parameters the model needs except the grid.
The main parameters are the grid size, that is how many grid lines there are in
the three directions. The number of sediment sizes is also an important
parameter. To generate the water surface it is necessary to know a downstream
water level, together with the water discharge and the Manning's friction
factor. These parameters are given on the G 1 and the W 1 data set in the
control file. If the control file does not exist, the user is prompted for
these parameters in a dialog box. The user can then later choose Write control
in the File option of the main menu, and get a control file written to the disk
(as control.new). This can then be edited according to the user's needs. Note
that only the most used parameters are written to the control.new file.

During the water flow calculations there are several parameters that can be
varied. These parameters affect the accuracy and the convergence of the
solution. These parameters can be modified while the water flow field is being
calculated. A dialog box with the parameters is invoked by choosing Waterflow
parameters from the Input Editor choice in the main menu.

The control file contains all other data that are necessary for the program.
SSIIM reads each character of the file one by one, and stops if a capital
T,F,G,I,S,N,B or W is encountered. Then a data set is read, depending on the
letter. A data set is here defined as one or more numbers or letters that the
program uses. This can for example be the water discharge, or the Manning's
friction coefficient. It is possible to use lower-case letters between the data
sets, and it is possible to have more than one data set on each line. Not all
data sets are required, but some are. Default values are given when a
non-required data set is missing. SSIIM controls the data sets in the control
file to a certain degree, and if an error is found, a message is written to the
boogie file and the program is terminated.

 Remember that the order of the data sets may be important. For example the G 1
data set should be early in the file. If the order of the data sets follows the
description given here, this should not be a problem.

 For the initialization and graphics, the following data sets are required:

G 1, G 3, W 1-2

For the sediment calculation, the following data sets are required:

S, I

For the water flow calculation by using MB-Flow, no data sets are required.

In addition, there are a number of optional data sets for each calculation.
These are described below.


ΓòÉΓòÉΓòÉ 4.1.1. T ΓòÉΓòÉΓòÉ

Title field. The following 30 characters are used in the graphics programs.


ΓòÉΓòÉΓòÉ 4.1.2. F 1 ΓòÉΓòÉΓòÉ

Debugging possibility. If the character that follows is a D, one will get a
more extensive print-out to the boogie file. If the character is a C, the
coefficients in the discretized equations will be printed to the boogie file.


ΓòÉΓòÉΓòÉ 4.1.3. F 2 ΓòÉΓòÉΓòÉ

Automatic execution possibility. Some parts of the program will be executed
directly after the initialization if a character is placed in this field. The
sub-programs will be executed in the order they are given. The possibilities
are:

 R Read the result file
 I Initialize the sediment calculations
 S Calculate sediment concentration
 W Start the multi-block water flow routine
 B Change the bed according to sediment calculation
 M Write result file
 P Use porosity in the calculation
 V Initialize water surface level
 X Read xcyc/koosurf files


ΓòÉΓòÉΓòÉ 4.1.4. F 4 ΓòÉΓòÉΓòÉ

Relaxation factor for second order interpolation of bed concentration, maximum
iterations for concentration calculations and convergence criteria for
suspended sediment calculation. The convergence criteria is given as allowable
flux deficit as part of inflowing sediments.

Defaults: relaxation: 0.5, iterations: 500, convergence criteria: 0.01.


ΓòÉΓòÉΓòÉ 4.1.5. F 6 ΓòÉΓòÉΓòÉ

Coefficients for formula for bed concentration. Default is van Rijn's
coefficients: 0.015, 1.5 and 0.3. If one uses this option, the sediment
transport formula given in dataset F 10 must be R, which is van Rijn's formula
is used as basis.


ΓòÉΓòÉΓòÉ 4.1.6. F 7 ΓòÉΓòÉΓòÉ

Run options. read 10 characters. If the following capital letters are included
this will mean:
 D Double the number of grid cells in streamwise direction in comparison to
what is given in the koordina file. Each cell is divided in two equal parts.
When this option is used for the whole geometry, the number of grid lines in
the streamwise direction (on the G 1 data set) must be multiplied with 2 and 1
must be subtracted.
 J Double the number of grid cells in the cross-streamwise direction. The same
procedure for the lines in the cross- streamwise direction (G 1 data set) is
required.
 I Inflowing velocities in the y-direction are set to zero.
 A Diffusion for sediment calculations in non-vertical direction is set to
zero.
 B Correction for sloping bed is used when calculating bed sediment
concentration.
 G Cell walls at outblocked area is not changed when there are changes in the
cells outside the block.
 V 90 degree turning of the plot seen from above (map).
 Z Vertical distribution of inflowing sediment is uniform.
 X Grid is read in from the "XCYC" file. This is only used in the
post-processor, and with presentation of results from Spider where the lines in
the k-direction are not vertical.
 C Inflowing and ouflowing water in default walls is set to zero. This means
that the water flow must be specified on the G 7 data sets.
 E Activate a routine that changes the flux on the wall if ap=0.
 P Use the porosity file


ΓòÉΓòÉΓòÉ 4.1.7. F 8 ΓòÉΓòÉΓòÉ

Maximum bed level change relative to water depth. This is controlled for all
the cells. Default: 0.1. This parameter is used to compute the time step for
the bed changes.


ΓòÉΓòÉΓòÉ 4.1.8. F 9 ΓòÉΓòÉΓòÉ

Factor that is used to change the turbulent viscosity of the inflowing water.
The factor is proportional to the turbulent viscosity. Default: 1.0.


ΓòÉΓòÉΓòÉ 4.1.9. F 10 ΓòÉΓòÉΓòÉ

Which sediment transport formula is used to calculate the concentration at the
bed. The following options are given:

 R van Rijn's formula
 E Engelund/Hansen's formula
 A Ackers/White's formula
 Y Yang's streampower formula
 S Shen/Hung's formula

Default: R.

Note that only the option R is fully tested.


ΓòÉΓòÉΓòÉ 4.1.10. F 11 ΓòÉΓòÉΓòÉ

Density of sediments and Shield's coefficient. Default: 2.65 and 0.047.


ΓòÉΓòÉΓòÉ 4.1.11. F 12 ΓòÉΓòÉΓòÉ

Schmidt's coefficient, which is a correction factor for deviation between the
turbulent diffusivity for sediment and water. Default: 1.0


ΓòÉΓòÉΓòÉ 4.1.12. F 15 ΓòÉΓòÉΓòÉ

An integer that determines how the law walls will be used in the cells which
borders both the wall and the bed. A value of 0 will make the program use wall
laws on both walls. A value of 1 will make the program only use wall laws on
the bed wall. For cases where the vertical dimensions are approximately the
same as the horizontal dimensions, a value of 0 is recommended. Default: 0.


ΓòÉΓòÉΓòÉ 4.1.13. F 16 ΓòÉΓòÉΓòÉ

Roughness coefficient which is used on the side walls and the bed. If not set,
the coefficient is calculated from the Manning's friction coefficient. The file
bedrough overrides this value for the bed cells.


ΓòÉΓòÉΓòÉ 4.1.14. F 18 ΓòÉΓòÉΓòÉ

Density current source. A float is read, and if it is above 10-6, the sediment
density term in the Navier-Stokes equation is added. The float is multiplied
with the density term, so a value of 1.0 is recommended when this term is
needed. Default 0.0 (the term is not used).


ΓòÉΓòÉΓòÉ 4.1.15. F 20 ΓòÉΓòÉΓòÉ

Repeated calculation option. An integer is read, and the calculation sequence
on the F 2 data set will be repeated this many times. Note that the graphical
view of the bedlevel changes will only appear on the last iteration when
sediment calculations are done. Also note that if a result file is read in the
F 2 data set, it is only read during the first iteration.


ΓòÉΓòÉΓòÉ 4.1.16. F 21 ΓòÉΓòÉΓòÉ

Relaxation coefficient for the Rhie and Chow interpolation. Normally a value
between 0.0 and 1.0 is used. When 0.0 is used the Rhie and Chow interpolation
will have no effect. When 1.0 is used the Rhie and Chow interpolation will be
used normally. Default 1.0.


ΓòÉΓòÉΓòÉ 4.1.17. F 22 ΓòÉΓòÉΓòÉ

Minimum porosity and relaxation factor for porosity calculations. Two floats.
Default 0.2 and 2.0.


ΓòÉΓòÉΓòÉ 4.1.18. F 24 ΓòÉΓòÉΓòÉ

 Turbulence model. An integer is read, which corresponds to the following
models:

 0 : standard k-Γûá model (default)
 7 : eddy viscosity = 0.11 * depth * shear velocity (Olsen, 1991)

 Note that only option 0 and 7 has been implemented, and that option 7 only
works for the two-dimensional calculation.


ΓòÉΓòÉΓòÉ 4.1.19. F 25 ΓòÉΓòÉΓòÉ

Porosity parameters. Four floats and one integer. The two first floats are
identical to the ones on the F 22 data set. The following two floats give the
porosity on the second and third level above the ground. These have default
values 0.5 and 0.8. These are used if the roughness height is larger than the
levels of the porosity in the porosity file. The effective porosity height is
set to maximum of bed cell height and roughness height. The last integer
determines the procedure for finding particle diameter in the porosity formula.
The following options are given: (default 0)

 0 : Maximum of roughness height and porosity height
 1 : Maximum of roughness height and 0.33 * porosity height
 2 : Equal to height of bed cell
 3 : Maximum of height of bed cell and porosity height


ΓòÉΓòÉΓòÉ 4.1.20. F 26 ΓòÉΓòÉΓòÉ

Volume fraction of sediments in deposits. One float is read. Default 0.5. If
the water content is 51 % in a fully saturated sample, the volume fraction will
be 0.49.


ΓòÉΓòÉΓòÉ 4.1.21. F 30 ΓòÉΓòÉΓòÉ

Bed concentration recalculation methods. Six integers are read. The first
integer determines which initial bed sediment grain size distribution is
present. The following possibilities are present:

 0 : Given by the user on the N data sets
 1 : Shield's graph method
 2 : Zero for all sizes

The second integer tells which method is used to recalculate the bed  sediment
grain size distribution. The following options are given:

 0 : No recalculation
 1 : Recalculation based on fluxes in/out of the bed cell
 2 : Recalculation based on deposition
 3-5 : Recalculation based on deposition and erosion

 Option 3 and 4 does not necessarily scale the sum of the fractions to unity,
if the sum is below unity. Option 5 does. Option 4 allows the sum of the
fractions to be above unity, whereas option 3 and five does not.

 Note that the method for recalculation of bed grain size distribution is still
on the experimental stage, and that the above options are not verified yet.

 The third integer invokes second order extrapolation of bed concentration if
it is 2.

 If the fifth integer is 2, it invokes routine that keeps the bed concentration
under the level of the inflowing concentration.

 Default: F 30 0 0 0 0 0 0 Note that six integers must be present, even if only
one or two are different from zero.


ΓòÉΓòÉΓòÉ 4.1.22. F 31 ΓòÉΓòÉΓòÉ

Two porosity coefficients are read. The coefficients are used for making the
porosity file. This is further described here  Default: F 31 0.8 0.8


ΓòÉΓòÉΓòÉ 4.1.23. F 33 ΓòÉΓòÉΓòÉ

Transient water flow parameters. A float and an integer is read. The float is
the time step. The integer is the number of inner iterations for each
iteration. Transient terms will be included in the equations if this data set
is present.


ΓòÉΓòÉΓòÉ 4.1.24. F 36 ΓòÉΓòÉΓòÉ

Transient free surface routine is invoked if the F 36 1 data set is present.
Note that this has not yet been fully implemented.


ΓòÉΓòÉΓòÉ 4.1.25. F 37 ΓòÉΓòÉΓòÉ

Transient sediment calculation is invoked if the F 37 1 data set is present.
Note that this has not yet been fully implemented.


ΓòÉΓòÉΓòÉ 4.1.26. F 38 ΓòÉΓòÉΓòÉ

Residual limit for when warning messages are written to the boogie file.
Default: 1.0e+7.


ΓòÉΓòÉΓòÉ 4.1.27. F 40 ΓòÉΓòÉΓòÉ

Turbidity current parameter. If this is unity the extra term in the Navier-
Stokes Equation are taken in that takes into account the effect of
gravitational forces on water that have higher density because of high sediment
concentration. If this is above 0.001, the term is still incorporated but
relaxed with the factor on the data set. Default 0.0.


ΓòÉΓòÉΓòÉ 4.1.28. F 41 ΓòÉΓòÉΓòÉ

Maximum scour depth for bed changes in meters.


ΓòÉΓòÉΓòÉ 4.1.29. F 42 ΓòÉΓòÉΓòÉ

Minimum level where the bed will not move under in meters.


ΓòÉΓòÉΓòÉ 4.1.30. F 43 ΓòÉΓòÉΓòÉ

Underflow parameter. An integer is read. If it is 1 the solver will check for
underflow errors and correct these. This procedure will cause SSIIM to run
slightly slower. The parameter can be used if the program halts with the system
underflow error. This is most often encountered when blocking out regions of
the flow. Default 0.


ΓòÉΓòÉΓòÉ 4.1.31. F 44 ΓòÉΓòÉΓòÉ

Two-dimensional flow calculation parameter. If 1 the two-dimensional
calculation will be used. If 0, the 3D calculation will be used. Default 0.


ΓòÉΓòÉΓòÉ 4.1.32. F 45 ΓòÉΓòÉΓòÉ

Transient Free Surface parameters. Three floats are read.

The first is a diffusion parameter for spreading of water flow elevation to the
corners of the cell. A small parameter will cause movements in the direction of
the flow. A larger value will give more movements in all directions. It is only
used when the flow is supercritical. Default 0.05.

The second float is an accelleration factor for speeding up a wave. When zero,
this has no effect. A factor of 1.0 may give higher speed. Default 0.0.

The third float is a damping parameter for obstacles in the flow. Default: 2.0,
which means no damping.


ΓòÉΓòÉΓòÉ 4.1.33. F 47 ΓòÉΓòÉΓòÉ

Interpolation parameter in meters. One float is read, which is used in the bed
interpolation routine that are called from the GridEditor. If the points given
in the geodata file are located a horizontal distance under the interpolation
limit, than the interpolation routine will use the exact value of the geodata
point instead of interpolating from surrounding points.

 Default: 0.05 m.


ΓòÉΓòÉΓòÉ 4.1.34. F 48 ΓòÉΓòÉΓòÉ

Parameter for interpolation of results. An integer is read. If 0, then a normal
result file will be written when this routine is invoked. If higher values are
given, the program will search for the interpol file. It will use this file to
write an interres file. If the value is 0, the bed levels will be written to
the interres file. If 2, the velocities, k and epsilon will be written to the
file. If 3, then sediment concentrations will be written. Default 0. Further
description of the interpol and interres files is given here

Note that the procedure for writing the interres file and this data set changed
from SSIIM version 1.3 to version 1.4.


ΓòÉΓòÉΓòÉ 4.1.35. F 50 ΓòÉΓòÉΓòÉ

Number of water quality constituents.


ΓòÉΓòÉΓòÉ 4.1.36. F 53 ΓòÉΓòÉΓòÉ

Print iterations. Four integers are read, which gives the interval for when
print-out to files are done. The first integer applies to the residual printout
to the boogie file. The second integer applies to writing the result file. The
third integer applies to writing data to the forcelog file. The fourth integer
applies to when data is written to the timeo file.

Default: F 53 100 100 1 1

This means that for example the result file is written each 100th iteration.


ΓòÉΓòÉΓòÉ 4.1.37. F 54 ΓòÉΓòÉΓòÉ

A float is read, which is a limit for the residual during the transient
calculation. When the maximum residual goes below this value, the inner
iterations end, and a new time step starts. Default 10e-7


ΓòÉΓòÉΓòÉ 4.1.38. F 55 ΓòÉΓòÉΓòÉ

Maximum allowable bed concentration. A float. Default 0.3.


ΓòÉΓòÉΓòÉ 4.1.39. F 56 ΓòÉΓòÉΓòÉ

Avalanche parameters. An integer and a float is read. If the integer is above
zero, an avalanche procedure will be invoked in the TSC calculation. This
routine checks the bed slope after each bed movement to see if it is above a
certain angle (of repose). If it is, then the bed slope will be adjusted to
become equal to the angle of repose. The float that is read is tan to the angle
of repose. Example: 1.0 is equal to an angle of repose of 45 degrees.

If all the grid lines at the bed is checked, and one is adjusted, it is
possible that a neighboring grid line to the adjusted line becomes steeper than
the angle of repose, because of the first adjustment. To prevent this, the
avalanche procedure is repeated a number of times. The number of times is given
by the first integer in the data set.

Default: This procedure is not invoked automatically.


ΓòÉΓòÉΓòÉ 4.1.40. F 58 ΓòÉΓòÉΓòÉ

TFS parameters. Four integers, i1-i4, and six floats, f1-f6, are read, which
controls the TFS calculation.

i1 removes the time term in the Navier-Stokes equations if it is 0. Default: 1.

i2 corrects the pressure so that it is always possitive if i2 is 1. Default 0.

i3 makes walls of outblocked regions move vertically according to the water
surface if it is 1. Default 0.

i4 will give more water level movements in the direction of the velocity vector
if i4 is 1. It will give equal movement in all direcions if it is 0. Default 1.

f1 is a diffusion factor for forward movement of water surface elevation
changes. If i4 is 1, and f1 is zero, all horizontal water surface movements are
in the direction of the velocity vector. If f1 is a large number, all movement
will be distributed equally in all directions, even if i4 is 1. Default: 0.02.

f2 is a damping coefficient for the side walls. If f2 is 2.0, there will be no
damping of the vertical water movement at the side walls. If f2 is 0.0, the
damping is so great the water surface will not move at all. Default 2.0.

f3 is a damping coefficient for the outblocked regions. Otherwise similar to
f2. Default 2.0.

f4 gives the influence of the water surface movement on the velocity in the
cell closest to the water surface. If f4 is 0, there will be no effect. If f4
is 1.0, the vertical velocity will be set equal to the velocity of the water
surface. (Note that f4 above 0 will give unphysical results for a steady flow
with sloping water surface)

f5 is a factor which includes a source term for the accelleration force from
the moving grid on the water in the cells. The term is multiplied with f5, so
that zero gives no effect of the term.

f6 is a smoothing factor for the water surface. Zero gives no smooting.

Summary of defaults: F 58 1 0 0 1 0.02 2.0 2.0 0.0 1.0 0.0

Note that the TFS routine and these parameters are still on an experimental
stage. When more research and testing is done, it will probably be possible to
remove several of the parameters as the influence of the various effect is
better understood.


ΓòÉΓòÉΓòÉ 4.1.41. F 59 ΓòÉΓòÉΓòÉ

Number of iterations in the Gauss-Seidel procedure. This is an integer which
will affect the convergence and speed of the program. A lower value will
increase the number of iterations pr. time, while slowing the relative
convergence pr. iteration. For some cases, a lower value has given decreased
computational time. Note that if the TDMA solver (K 10 data set) is used, then
the F 59 data set will have no effect. Default: 10.


ΓòÉΓòÉΓòÉ 4.1.42. F 60 ΓòÉΓòÉΓòÉ

Two integers are read. If the first integer is unity, an algorithm is invoked,
where the concentration in the bed cell is extrapolated from what was given by
van Rijn's formula by using the Hunter-Rouse equation for the suspended sedimen
concentration profile.

If the second integer is unity, the bedform roughness will be taken into
account when calculating the sediment concentration. Note that this is not
tested yet.

Default: F 60 0 0


ΓòÉΓòÉΓòÉ 4.1.43. G 1 ΓòÉΓòÉΓòÉ

xnumber, ynumber, znumber and lnumber. There are four integers that show the
number of grid lines in the streamwise, cross-streamwise and vertical
direction. lnumber is the number of sediment sizes. This data set must be
present in the control file. The program will read these values and allocate
space for the arrays accordingly.


ΓòÉΓòÉΓòÉ 4.1.44. G 3 ΓòÉΓòÉΓòÉ

Vertical distribution of grid cells. This dataset must be present in the file.
A number of floats are read; equally many as grid lines in the vertical
direction. The first number is 0 and the last is 100 (%). If there for example
are 4 grid lines in the vertical direction, and the first cell is has a height
of 25 % of the depth, the second cell has a height of 40 % of the depth and the
third (top) cell has a height of 35 % of the depth, the following data set is
used:

G 3 0.0 25.0 65.0 100.0


ΓòÉΓòÉΓòÉ 4.1.45. G 5 ΓòÉΓòÉΓòÉ

Sediment sources. Six integers and lnumber floats are read. The integers
indicate a region of the grid. The first two are in the streamwise direction,
the following two are in the cross-stream direction and the two last integers
indicate the vertical direction. The following floats gives the sediment
concentration in volume fractions.

Example: Sediment concentration 0.001 flows into the top of the geometry n an
area given by the following cells: j=2 to j=4 and i=3 to i=5. It is assumed
that there are 11 grid lines in the vertical direction. This gives the
following data set:

G 5 3 5 2 4 11 11 0.001


ΓòÉΓòÉΓòÉ 4.1.46. G 6 ΓòÉΓòÉΓòÉ

Data set for calculating water surface location with an adaptive grid. Three
integers and two floats:

  iSurf:
  jSurf:
  kSurf:

These are three integers that indicate three grid lines. This point is a
reference point, and it is not moved. In the present implementation, kSurf have
to be equal to znumber + 1. If not, a warning message is sent to the boogie
file, and kSurf is set to znumber + 1. The computations continue afterwards.

  RelaxSurface:

 This is a float that relaxes the estimation of the increment to the new
recalculated water surface. Recommended values are between 0.5 and 0.95.

  ConvSurface:

 This float sets the limit for when the water surface should be recalculated.
The water surface will be updated when the maximum residual of the equations
are below this parameter. Recommended value: 0.01 - 1.0


ΓòÉΓòÉΓòÉ 4.1.47. G 7 ΓòÉΓòÉΓòÉ

This data set specifies water inflow on geometry sides, bed or top. Each
surface is given on one G 7 dataset. It is possible to have up to 19 G 7
datasets.

On each dataset, seven integers and four floats are read. The names of these
variables are:

 G 7 type, side, a1, a2, b1, b2, parallel, update, discharge, Xdir, Ydir, Zdir

 Each variable is explained in the following:

 - type:  1: outflow, 0: inflow.
 - side:  1: plane i=1
     -1: plane i=xnumber,
      (cross-streamwise plane)
      2: plane j=1
     -2: plane j=ynumber,
      (streamwise plane)
      3: plane k=1
     -3: plane k=znumber
      (horizontal plane)
 - a1,a2,b1,b2: four integers that determine the limits of the
      surface. An example is shown in the figure.


 - parallel: direction of the flow:
   0: normal to surface
   1: parallel to grid lines normal to surface
   2: direction is specified (vector directions)
 - update: 0 for not update, 1 for update.
  (only partly implemented)
 - discharge:  discharge in qm/s. Note that the sign of the
    discharge must correspond with the direction of the
    desired flow velocity. Positive discharges indicate
    discharges in positive directions.
 - Xdir:   direction vector in x-direction
 - Ydir:   direction vector in y-direction
 - Zdir:   direction vector in z-direction

 Example: G 7 0 1 2 11 2 11 0 0 32.0 1.0 0.0 0.0

 This example specifies inflow in the most upstream cross-section. The inflow
area is from cell no. 2 to cell no. 11 in both cross- streamwise and vertical
direction. The flow direction is normal to the cross-section. The discharge is
32 cubic meters/second.

 The parameter "side" can be used to specify flux on sections that have been
"amputated" by the multi-block procedure. The parameter side is then evaluated
as the number of the block plus 10. Example: A geometry with one multi-block
that starts at node i=30. To specify flux on wall i=29, use the G7 data set
with the parameter "side" set to 11 (10+1).

Remember to define the walls of the boundary that when this dataset is used.
This must be done on the W 4 data set. If inflow through a wall is specified
with the G 7 data set, the wall must be removed with the W 4 data set.


ΓòÉΓòÉΓòÉ 4.1.48. G 8 ΓòÉΓòÉΓòÉ

Values for initial velocities. Up to 19 data G 8 data sets can be used. Six
integers are read first to specify the volume that is being set. Then three
floats are read, which gives the velocities in the three directions.

 G 8  i1  i2  j1  j2  k1  k2  U  V  W


ΓòÉΓòÉΓòÉ 4.1.49. G 11 ΓòÉΓòÉΓòÉ

Source terms for the velocity equations. Six integers and two floats.

 i1,i2,j1,j2,k1,k2, source, relax

The first six integers give the cells that are influenced by the source term.
The source variable is the form factor times a diameter of a cylinder in the
cell. The relaxation variable is recommended set between 1.0 and 2.0


ΓòÉΓòÉΓòÉ 4.1.50. G 12 ΓòÉΓòÉΓòÉ

Sediment source for multi-block border. This is used where there is inflow of
sediments in a branch of a block that is cut of. An integer is first read,
which tells the number of the block. Then lnumber floats are read, which is
inflow of sediments for each size. This is given in kg/s. The option is not
fully tested yet.


ΓòÉΓòÉΓòÉ 4.1.51. G 13 ΓòÉΓòÉΓòÉ

Outblocking option that is used when a region of the geometry is blocked out by
a solid object. An integer is read first, which determines which sides the wall
laws will be applied on. The following options are possible:

 0: No wall laws are specified
 1: Wall laws are used on the sides of the block
 2: Wall laws are used on the sides and the top of the block
 3: Wall laws are used on the sides, the top and the bottom of the block

 Six integers are then read, i1,i2,j1,j2,k1,k2. These integers define the cells
of the block. The two first integers are the first and the last cell in the
i-direction. The next two integers are the first and the last cell in the
j-direction. The last two integers are the first and the last cell in the
vertical direction.

When making blocks, note that there must be at least two free cells (not
blocked out) between each block or to the wall. It is recommended to use more
free cells than two, to resolve the flow pattern between the blocks.

Up to 19 G 13 data sets can be used.


ΓòÉΓòÉΓòÉ 4.1.52. G 14 ΓòÉΓòÉΓòÉ

Debug dump option, where a variable in a cell is written to the boogie file.
Four integers are read. The first integer indicate which equation. Velocities
in x,y and z directions are denoted 1,2 and 3, respectively. 5 and 6 are used
for k and Γûá, respectively.

The next three integers are cell indexes i,j and k.

Example: G 14 1 3 4 6 causes velocity in x-direction for cell i=3, j=4 and k=6
to be written to the boogie file for each iteration.

Up to 29 G 14 data sets can be used.


ΓòÉΓòÉΓòÉ 4.1.53. G 15 ΓòÉΓòÉΓòÉ

Scaling factor for mouse location in graphics routines. Default 1.0


ΓòÉΓòÉΓòÉ 4.1.54. G 16 ΓòÉΓòÉΓòÉ

Local vertical distribution of grid cells. This data set can be used when a
different distribution of grid cells than what is given on the G 3 data set is
wanted in some parts of the geometry. Four integers are read first. These tells
which area are affected by the changed distribution. Then znumber floats are
read, similarly to what is on the G 3 data set.

Example: G 16 2 3 1 4 0.0 50.0 75.0 100.0 when znumber is 4, gives the new
distribution for the eight vertical lines i=2 to i=3 and j=1 to j=4.

Up to 20 G 16 data sets can be used.


ΓòÉΓòÉΓòÉ 4.1.55. G 18 ΓòÉΓòÉΓòÉ

Specification of inflow of water quality constituents. Seven integers and two
floats are read. The first six integers specify a surface where the inflow is.
The first two integers are the streamwise index, the next two the cross-
streamwise index and the last 5th and 6th integers specify the vertical index.
Example: Inflow through the upstream boundary (i=1), on cross-streamwise cell
index j=2 to 4 and vertical cell k=3 to 5 gives the following six numbers:  G
18 1 1 2 4 3 5 ....  Note that one of the three pairs have to be identical to
define a surface.

 The seventh integer is an idex to specify the water quality consituent. Note
that 0 is used for the first constituent, 1 for the second etc.

 The eighth number, or first float, is the value of the water quality
constituent at the boundary.

 The ninth number, or second float, is the time when the water quality
constituent start flowing into the geometry. Note that if two G 18 data sets
are given at the same location for the same variable, the one with the higher
time value will overwrite the inflow data for the data set with the lower time
value. This makes it possible to specify a discrete time series of inflow.

A maximum of 100 G 18 data sets can be used.


ΓòÉΓòÉΓòÉ 4.1.56. G 19 ΓòÉΓòÉΓòÉ

OpenGL 3D surfaces parameters. One surface is described on each G 19 data set.
Up to 50 G 19 data sets can be used.

Each data set consist of eight integers. The first integer specifies the number
of the grid line. The second integer is an index showing the main direction of
the grid surface. The following options are possible:

1: cross-section
2: longitudinal profile
3: plan view

 The following four integer defines the corners of the surface. The last two
integers are presently not used for anything, but they must be given.

Example: G 19 11 3 2 5 2 6 0 0

This gives a surface along the grid surface k=11, from i=2 to 5, and j=2 to 6.

If no G 19 data sets are given, a default data set is used this is:

G 19 1 3 2 xnumber 2 ynumber 0 0

This will give the bed of the geometry. The parameters xnumber and ynumber are
given on the G 1 data set, and is the number of grid lines in the streamwise
and cross-streamwise direction.


ΓòÉΓòÉΓòÉ 4.1.57. H 1 ΓòÉΓòÉΓòÉ

This data set is used for plotting a color graphics map where the plotted
parameter is the absolute value of the velocity. The user chooses different
colors and fill pattern according to the variable.

 An integer is first read, which tells how many different colors and fill
patterns are wanted. Then a floating point, v1, is read which marks the upper
boundary for the variable. Then two integers are read. The first integer, i1,
tells what color is used, and the second integer,j1, tells what fill pattern is
used. All areas that have a value below v1 will be filled with the color i1 and
pattern j1. Up to 20 points can be used. Example:

 H 1 3 0.01 1 1 0.1 2 2 1.0 3 3

 The elements which have an absolute velocity under 0.01 m/s will be filled
with the color no. 1 and fill pattern 1. The elements with absolute velocity
between 0.01 and 0.1 will be filled with color 2 and fill pattern 2.

 The numbers of the different colors and fill patterns are given below:

 No.  Color

 1 Green
 2 Blue
 3 Black
 4 Cyan
 5 Magenta
 6 Brown
 7 Red
 8 Yellow
 9 Pale gray
 10 Dark gray
 11 Dark blue
 12 Dark red
 13 Dark magenta
 14 Dark green
 15 Dark cyan
 16 White

 The numbers of the different density patterns are given below:

 No.  Patten

 1 Blank
 2 Density1, light
 3 Density2
 4 Density3
 5 Density4
 6 Density5
 7 Density6
 8 Density7
 9 Density8, dark
 10 Diagonal lines, SW-NE, narrow spacing
 11 Diagonal lines, SW-NE, wide spacing
 12 Diagonal lines, NW-SE, narrow spacing
 13 Diagonal lines, NW-SE, wide spacing
 14 Horizonal lines
 15 Vertical lines
 16 Solid


ΓòÉΓòÉΓòÉ 4.1.58. H 2 ΓòÉΓòÉΓòÉ

Color map plotting for water depth instead of velocity. Otherwise it is the
same as the H 1 data set.


ΓòÉΓòÉΓòÉ 4.1.59. H 3 ΓòÉΓòÉΓòÉ

Color map plotting for sediment size instead of velocity. Otherwise it is the
same as the H 1 data set.


ΓòÉΓòÉΓòÉ 4.1.60. H 4 ΓòÉΓòÉΓòÉ

Color map plotting for bed shear stress instead of velocity. Otherwise it is
the same as the H 1 data set.


ΓòÉΓòÉΓòÉ 4.1.61. H 5 ΓòÉΓòÉΓòÉ

Color map plotting for turbulent kinetic energy. Otherwise it is the same as
the H 1 data set.


ΓòÉΓòÉΓòÉ 4.1.62. H 6 ΓòÉΓòÉΓòÉ

Color map plotting for sediment concentration. Otherwise as H 1.


ΓòÉΓòÉΓòÉ 4.1.63. H 14 ΓòÉΓòÉΓòÉ

Color map plotting for bed level changes. Otherwise as H 1.


ΓòÉΓòÉΓòÉ 4.1.64. L ΓòÉΓòÉΓòÉ

Specification of isoline values for ContourMap plot. First, an integer is read,
which gives the number of isolines. Then, this number of floats are read. The
floats specify the isolines. Example:

 L 6  55.0 56.0 57.0 58.0 59.0 60.0

 If the geometry has bed levels between 55 and 60 meters, and the user chooses
bed levels from the graphics options, a contour map of the bed levels will be
displayed. There will be contour lines for each meter, from 55 to 60 meters.

Default: The program finds the maximum and minimum value of the variable in the
field, and uses 5 lines located between the values.

If more than 5 lines are displayed, all lines will be black. Otherwise each
line will have different color.

Note that sometimes there may be errors in the contouring, if the contour line
and the value are identical. This can often be the case for plotting bed
levels. To avvoid this problem, add a very small value to the values on the L
data set. For example, if the above data set is used and there is a problem for
the 57.0 contour line because the bed level at one of the grid intersections
are 57.0, change the data set to:

 L 6 55.0 56.0 57.0001 58.0 59.9 60.0


ΓòÉΓòÉΓòÉ 4.1.65. P 2 ΓòÉΓòÉΓòÉ

Five floating points that give scaling for the graphical presentation. The
first three gives scales in streamwise, cross-streamwise and vertical
direction. The fourth and fifth give movements in left-right and vertical
direction. Defaults: 1.0 for the scales, and 0.0 for the movements.


ΓòÉΓòÉΓòÉ 4.1.66. P 3 ΓòÉΓòÉΓòÉ

Four integers that give initial location of the graphical plots in streamwise,
cross-streamwise and vertical direction, and sediment fraction number.


ΓòÉΓòÉΓòÉ 4.1.67. P 4 ΓòÉΓòÉΓòÉ

A character that indicates initial type of plot. "g" gives the grid, "v" gives
velocity lines, "V" gives velocity vectors, "c" gives concentration.


ΓòÉΓòÉΓòÉ 4.1.68. W 1 ΓòÉΓòÉΓòÉ

Manning's number, discharge and downstream waterlevel. This dataset must be
present in the file. The parameters given here are used to generate the
waterlevel for the calculations using a standard backwater calculation.


ΓòÉΓòÉΓòÉ 4.1.69. W 2 ΓòÉΓòÉΓòÉ

Water surface initialization array of integers. The first integer tells how
many numbers there are in the array. The next numbers tell which cross-
sections are going to be used in the initialization of the water surface of the
grid. The integers must be given in rising order, and start with 1. This
dataset must be present in the file.


ΓòÉΓòÉΓòÉ 4.1.70. W 3 ΓòÉΓòÉΓòÉ

Specification of multiple blocks for the multi-block water flow module. First
an integer that indicates the number of extra blocks is given. The maximum
value is 9. Then two integers for each extra block are given. The first integer
tells where the block is cut off. The second integer tells where the block is
added. If the second integer is negative, the block is added on the left side
of the main block. Otherwise it is added on the right side of the block. This
is explained with an example on the figure below. The corresponding dataset
would be: W 3 1 10 -5


ΓòÉΓòÉΓòÉ 4.1.71. W 4 ΓòÉΓòÉΓòÉ

Specification of extra walls for the multi-block water flow module. Seven
integers have to be given for each wall. There can be up to 29 walls, and each
wall is described on one W 4 data set.

 The variable names are:

W 4 dir,posneg,node,a1,a2,b1,b2

 The first integer, dir, indicates the plane. 1 is the j-k plane
(cross-section), 2 is the i-k plane (longitudinal section) and 3 is the i-j
plane (seen from above).

 The second integer, posneg, indicates if the wall is in the positive or
negative direction of the node. The coordinates are given for nodes. 1 or -1 is
given. If 0 is given, a previously set wall is deleted.

 The third integer is the number of the node plane.

 An example is given in the figure below. The figure shows the i-j plane. The
wall is to be given on node i=4. If the second integer, posneg, is 1, then wall
laws are applied on the wall upstream of node 4, in the negative i-direction.
If posneg = -1, then the wall laws are applied on node 4 if the cell in the
downstream i-direction (line i=3) is a wall.

The four following integers are indexes a1,a2,b1,b2, which gives the
two-dimensional coordinates for the corner points of the part of the plane that
is described. The four integers are the same as given on the G 7 data set.


ΓòÉΓòÉΓòÉ 4.1.72. W 5 ΓòÉΓòÉΓòÉ

Different Manning's values than the default value for cross-sections. An
integer is first read, which tells how many cross-sections are read. Then an
integer and a float is read for each cross-section. The integer tells which
cross-section is changed, and the float tells the Manning's value. Several W 5
data sets can be used.


ΓòÉΓòÉΓòÉ 4.1.73. W 6 ΓòÉΓòÉΓòÉ

NoMovePoint - a point which is used in the GridEditor. Two integers are read,
which is the numbers of the i and j grid lines. The intersection of these lines
are not moved by the elliptic grid generator. One W 6 data set is required for
each NoMovePoint. Maximum 199 points can be used.

The W 6 data set is usually generated by the Grid Editor.


ΓòÉΓòÉΓòÉ 4.1.74. W 7 ΓòÉΓòÉΓòÉ

Attraction point used in the GridEditor. Each W 7 data set represents
attraction to one grid line or point. Maximum 199 attraction points can be
used. An integer is read first which tells the type of attraction. The
following options are given:

 0: Point attraction in i-direction
 1: Point attraction in j-direction
 2: Line attraction in i-direction
 3: Line attraction in j-direction

 Then two integers are read, which tells which grid line intersection the
attraction is towards. For the line attraction, only one of the integers are
used. Then the two attraction parameters are read, which are floats.

 The W 7 data set is normally generated by the Grid Editor.


ΓòÉΓòÉΓòÉ 4.1.75. S ΓòÉΓòÉΓòÉ

Integer that gives the number of the sediment fraction, float that gives the
size of the sediments for these fraction, float that gives the fall velocity
for the fraction.

 There must be lnumber datasets like this in the file, as long as sediment
concentration is to be calculated. All numbers are given in SI units, that is,
the grain size is given in meters and the fall velocity is given in
meters/second. This data set must be present when sediment transport is
calculated.

 This dataset defines the grain sizes that are used in the program. Note that
this applies for both the grain sizes in the bed and in the suspended sediment
calculation.

The grain sizes should be numbered from 1 to lnumber, where size 1 is the
coarsest size, and the following sizes have decreasingly smaller diameter.


ΓòÉΓòÉΓòÉ 4.1.76. N ΓòÉΓòÉΓòÉ

These data sets define different grain size distributions for the sediments
that are in the bed when the calculation starts.

 Maximum 10 different samples can be used.

 Each sample has its own number. This starts with zero, and increases
sequentially to the total number of samples minus one.

 First, an integer for the number of the sample is given. The second integer
shows which size is described. The third number is a float, which gives the
fraction of the size in the sample. It is required to have lnumber N data sets
for each sample. These data sets must be present when sediment transport is
calculated.

 The number of N datasets that is required is:

 (number of grain size distributions) x (number of sediment sizes)

 Note that if only deposition is calculated, it is not necessary to specify the
N data sets. However, if the data sets are specified, the program will control
that the sum of the fractions are unity.


ΓòÉΓòÉΓòÉ 4.1.77. B ΓòÉΓòÉΓòÉ

This data set gives where the samples (from the N - data sets) are placed in
the geometry before the calculation starts.

The first integer indicates the number of the sample. The four following
integers give the number of the corner cells on a rectangle of the bed. The
sample is placed on the bed from i=second integer to i= third integer and
j=fourth integer to j=fifth integer. A B data set overwrite previous B
datasets.

The dataset B 0 0 0 0 0 tells that sample no. 0 covers the whole bed.


ΓòÉΓòÉΓòÉ 4.1.78. I ΓòÉΓòÉΓòÉ

Inflowing sediments. First integer shows which sediment fraction is simulated.
Second number is a float that is the amount of inflowing sediment of this size
in kg/s. lnumber of these data sets must be present when sediment
concentrations are calculated.  Note that the I dataset follows the sizes on
the S data set, but it has nothing to do with the N and B data sets.


ΓòÉΓòÉΓòÉ 4.1.79. K 1 ΓòÉΓòÉΓòÉ

Number of iterations for flow procedure and number that determines the minimum
iterations between updates of water surface. Two integers. Default:  K 1 40000
50000


ΓòÉΓòÉΓòÉ 4.1.80. K 2 ΓòÉΓòÉΓòÉ

Two integers that indicate if laws of the wall are being used. The first
integer applies to the side walls. The second integer applies for the surface.
0 is used for wall laws, and 1 for free surface. Wall laws are always used for
the bed, if not changed by the W 4 data set. Default: 0 1.


ΓòÉΓòÉΓòÉ 4.1.81. K 3 ΓòÉΓòÉΓòÉ

Relaxation factors. Six floats. For the three velocity equations, the pressure
correction equation and the k and Γûá equation.

Default:  K 3 0.8 0.8 0.8 0.2 0.5 0.5


ΓòÉΓòÉΓòÉ 4.1.82. K 4 ΓòÉΓòÉΓòÉ

Number of iteration for each equation. Six integers.

Default:  K 4 1 1 1 5 1 1


ΓòÉΓòÉΓòÉ 4.1.83. K 5 ΓòÉΓòÉΓòÉ

Block-correction index for each equation. Six integers. If 0, no block-
correction. If 1, the block-correction is used.

Default:  K 5 0 0 0 0 0 0  Note that the block-correction may not work with the
SOU scheme.


ΓòÉΓòÉΓòÉ 4.1.84. K 6 ΓòÉΓòÉΓòÉ

Six integers are read which determines whether the SOU or POW scheme is used.
If 0 POW is used, if 1, SOU is used. Note that presently the multi- block flow
module may not converge completely when the SOU scheme is used with multiple
blocks. This may be due to a bug. SOU will work if there is only one block.

Note that the flow module will always use the POW scheme for the
pressure-correction equation.

Default:  K 6 0 0 0 0 0 0


ΓòÉΓòÉΓòÉ 4.1.85. K 9 ΓòÉΓòÉΓòÉ

A character deciding whether SIMPLE or SIMPLEC is used. Y= SIMPLE, N = SIMPLEC.
Default: Y


ΓòÉΓòÉΓòÉ 4.1.86. K 10 ΓòÉΓòÉΓòÉ

A character that decides which solver is used. Y = Gauss-Seidel solver, N =
TDMA solver. Default: Y


ΓòÉΓòÉΓòÉ 4.1.87. Q ΓòÉΓòÉΓòÉ

There are two types of Q data sets. One is the Q 0 data set, which gives the
name of the variable. The other type specifies the source term in the
convection-diffusion equations.


ΓòÉΓòÉΓòÉ 4.1.88. Q 0 ΓòÉΓòÉΓòÉ

The Q 0 data set specifies the name of the constituent. This is used in the
graphics presentations. First, an integer is specified. This is the number
identifying the water quality constituents. Note that 0 is used for the first
constituent, 1 for the second etc. Example:  Q 0 0 temperature  Note that
lower-case letters must be used, and maximum 40.


ΓòÉΓòÉΓòÉ 4.1.89. Q 1 ΓòÉΓòÉΓòÉ

Q 1 specifies a biochemical source. First, an integer is read, identifying
which water quality constituent the source is applied to. Note that 0 is used
for the first constituent, 1 for the second, etc. Then a float is read, which
is a constant in the equation.  Example:  Q 1 0 0.001


ΓòÉΓòÉΓòÉ 4.1.90. Q 2 ΓòÉΓòÉΓòÉ

Q 2 specifies a biochemical source. First, an integer is read, identifying
which water quality constituent the source is applied to. Then a new integer is
read, which identifies a variable in the source term. Then a float is read,
which is multiplied with the variable.

Example:  Q 2 0 2 0.001

If variable 0 is oxygen and variable 2 is temperature, the example means that a
source term for the oxygen is that for all the cells there is a source term
equal to 0.001 times the temperature.


ΓòÉΓòÉΓòÉ 4.1.91. Q 3 ΓòÉΓòÉΓòÉ

Q 3 specifies a biochemical source. First, an integer is read, identifying
which water quality constituent the source is applied to. Then two integers are
read, specifying two variables. Then a float is read, which is multiplied with
the variables.

Example:  Q 3 3 2 1 -0.002

If variable 3 is algae, variable 2 is nitrogen and variable 1 is temperature,
then the data set specifiecs a negative source term for algae as 0.002
multiplied with the nitrogen concentration multiplied with the temperature.


ΓòÉΓòÉΓòÉ 4.1.92. Q 1001 ΓòÉΓòÉΓòÉ

Q 1001 specifies a biochemical source for the surface cells. First, an integer
is read, identifying which water quality constituent the source is applied to.
Note that 0 is used for the first constituent, 1 for the second, etc. Then a
float is read, which is a constant in the equation.  Example:  Q 1001 0 0.001


ΓòÉΓòÉΓòÉ 4.1.93. Q 1002 ΓòÉΓòÉΓòÉ

Q 1002 specifies a source for the surface cells. First, an integer is read,
identifying which water quality constituent the source is applied to. Then two
floats are read. The source term is : float1 * ( float2 - variable ).

Example:  Q 1002 0 0.001 23.0

This term can be used for calculation of temperature fluxes across the water
surface, where the first float is the heat exchange coefficient for the water
surface (0.001) and the second float is the air temperature (23 degrees).


ΓòÉΓòÉΓòÉ 4.1.94. Q 1003 ΓòÉΓòÉΓòÉ

Q 1003 specifies a biochemical source for the surface cells. First, an integer
is read, identifying which water quality constituent the source is applied to.
Then two integers are read, specifying two variables. Then a float is read,
which is multiplied with the variables.

Example:  Q 1003 3 2 1 -0.002

If variable 3 is algae, variable 2 is nitrogen and variable 1 is temperature,
then the data set specifiecs a negative source term for algae as 0.002
multiplied with the nitrogen concentration multiplied with the temperature.
This is only applied to the surface cells.


ΓòÉΓòÉΓòÉ 4.1.95. Q 1012 ΓòÉΓòÉΓòÉ

Q 1012 specifies a biochemical source for the surface cells. First, an integer
is read, identifying which water quality constituent the source is applied to.
Then a new integer is read, which identifies a variable in the source term.
Then a float is read, which is multiplied with the variable.

Example:  Q 1012 0 2 0.001

If variable 0 is oxygen and variable 2 is temperature, the example means that a
source term for the oxygen is that for all the surface cells there is a source
term equal to 0.001 times the temperature.


ΓòÉΓòÉΓòÉ 4.1.96. Q 2001 ΓòÉΓòÉΓòÉ

Q 2001 specifies a biochemical source for the bed cells. First, an integer is
read, identifying which water quality constituent the source is applied to.
Note that 0 is used for the first constituent, 1 for the second, etc. Then a
float is read, which is a constant in the equation.  Example:  Q 2001 0 0.001


ΓòÉΓòÉΓòÉ 4.1.97. Q 2002 ΓòÉΓòÉΓòÉ

Q 2002 specifies a biochemical source for the bed cells. First, an integer is
read, identifying which water quality constituent the source is applied to.
Then a new integer is read, which identifies a variable in the source term.
Then a float is read, which is multiplied with the variable.

Example:  Q 2002 0 2 0.001

If variable 0 is oxygen and variable 2 is temperature, the example means that a
source term for the oxygen is that for all the bed cells there is a source term
equal to 0.001 times the temperature.


ΓòÉΓòÉΓòÉ 4.1.98. Q 2003 ΓòÉΓòÉΓòÉ

Q 2003 specifies a biochemical source applied only to the cells close to the
bed. First, an integer is read, identifying which water quality constituent the
source is applied to. Then two integers are read, specifying two variables.
Then a float is read, which is multiplied with the variables.

Example:  Q 2003 3 2 1 -0.002

If variable 3 is algae, variable 2 is nitrogen and variable 1 is temperature,
then the data set specifiecs a negative source term for algae as 0.002
multiplied with the nitrogen concentration multiplied with the temperature,
only for the bed cells.


ΓòÉΓòÉΓòÉ 4.2. The boogie file ΓòÉΓòÉΓòÉ

 This is a file that shows a print-out of intermediate results from the
calculations. It also shows parameters as average water velocity, shear stress
and water depth in the initialization. Trap efficiency and sediment grain size
distribution is also written here. If errors occur, an explanation is also
often written to this file before the program stops. The file contains the data
that is normally written to the screen in a DOS program.

 The option D on the F 1 data set will give additional print-out to the file.

 Initially in the file it is written how much memory that is occupied by the
arrays that are dynamically allocated. To estimate the total recommended memory
requirement for SSIIM, add 1.2 MB to this value.

 A table then follows, which shows the cross-sectional area, hydraulic radius,
average velocity and water level at the cross-sections that have been used for
initializing the water surface. If the option D on the F 1 data set is used,
this information is written for all the cross-sections additionally. Then a
table of waterlevels for all cross-sections follows:

Loop1,iter,area,radius,velocity,waterlevel: 12 1.002389e+00 1.002389e+00 9.976163e-01
1.002390e+00
Loop1,iter,area,radius,velocity,waterlevel: 11 1.001588e+00 1.001588e+00 9.984146e-01
1.001589e+00
Waterlevel = 1.000398 meters for cross-section i = 10
Waterlevel = 1.000797 meters for cross-section i = 9
Waterlevel = 1.001195 meters for cross-section i = 8

 If SSIIM terminates and the boogie file contains the following message: Error,
negative areas for cell i=13, j=2, or some other combinations of i and j, then
there is an error in the koordina file. The indexes denote the cell number, so
for i=13, j=2, the x and y coordinates for the following grid line
intersections should be checked: (13,2); (13,1); (12,2) amd (12,1).

 If the MB-flow module is used, the residual norms are written. Then follows a
sequence of two lines for each iteration of MB-flow. An example with four
iterations is shown below:

Iter: 5, Resid: 1.69e-05 4.10e-06 2.73e-05 1.17e-04 1.38e-02 1.13e-02
Cont: 9.23e-08, DefMax: 1.65e-03, U,V,W(96,7,20): 6.40e-01 -5.14e-03 5.76e-02
Iter: 6, Resid: 1.62e-05 3.85e-06 2.62e-05 1.10e-04 1.31e-02 1.08e-02
Cont: 9.23e-08, DefMax: 1.56e-03, U,V,W(96,7,20): 6.40e-01 -5.14e-03 5.76e-02
Iter: 7, Resid: 1.57e-05 3.65e-06 2.50e-05 1.04e-04 1.25e-02 1.03e-02
Cont: 9.23e-08, DefMax: 1.48e-03, U,V,W(96,7,20): 6.40e-01 -5.14e-03 5.76e-02
Iter: 8, Resid: 1.51e-05 3.46e-06 2.38e-05 9.86e-05 1.18e-02 9.77e-03
Cont: 9.23e-08, DefMax: 1.41e-03, U,V,W(96,7,20): 6.40e-01 -5.14e-03 5.76e-02

 The first line has the word "Iter" at first. Then an integer follows, which
shows the number of the iteration. In the example above this runs from
iteration number 5 to 9. Then the residuals for the six equations are shown.
The x,y and z velocity equations are first, then the pressure equation and the
k and epsilon equation follow.  All these must be under 0.001 before the
solution has converged.

 The second line starts with the word "Cont". Then a floating point value is
shown. This is the sum of all the water inflow and outflow in the geometry.
This should be a very low value, typically under 10E-7. If a larger value is
given, check the boundary conditions. Then the word "DefMax" is written. The
residual for the cell with largest water continuity defect is then written. The
indexes for this cell are then written, with the velocities in the three
directions for this cell. In iteration 9 for the example above, the maximum
water continuity defect was 1.41e-3 kg/s for cell i=96, j=7, k=20. The velocity
in the x-direction for this cell was 0.64 m/s, the velocity in the y direction
was -5.14 mm/s and the velocity in the vertical direction was 5.76 cm/s.

 If 3D changes in the water surface elevation is calculated, the water surface
elevations along the centerlines in the two horizontal directions are written
to the boogie file. This is done for each update. An example of some of these
results is shown below:

WL(20,1) = 1.012947e+00
WL(20,2) = 1.012427e+00
WL(20,3) = 1.011113e+00
WL(20,4) = 1.009520e+00
WL(20,5) = 1.007900e+00

If the sedimentation calculation is used, the fluxes through the four side
walls and the trapped sediments are written for each size. This is written for
each 100th iteration. An example is shown below:

Trap efficiency after 24700 iter: all values in kg/s
 l=1: Trapped: 230.015, Fluxes (I1,I2,J1,J2): 229.843, 2.95575e-20, 0, 0 Resid: 0.000750
 l=2: Trapped: 485.265, Fluxes (I1,I2,J1,J2): 499.657, 85.56, 0, 0 Resid: 0.142433
 l=3: Trapped: -2617.23, Fluxes (I1,I2,J1,J2): 269.815, 3489.59, 0, 0 Resid: 2.233171

 Three sizes are given in the example. For size 2 the inflow is 499.657 kg/s,
the outflow is 85.56 kg/s and 485.256 kg is trapped. The residual is the
continuity defect divided by the inflow. The convergence criteria is given on
the F 4 data set. The solution is converged when the average residual is under
the convergence criteria.

 After the sedimentation calculation has finished, the time step is written. A
further explanation of the time step is given in [4].

 If the bed changes are calculated this is also written to the file. The bed
changes are given in meters. An example is given below:

BedMove(10,8) = 1.009495e-03 meters
BedMove(10,9) = 1.030140e-03 meters
BedMove(10,10) = 1.019934e-03 meters

 In the example, the deposition in cell i=10, j=10 causes the bed to rise 1.02
mm during the given time step.

 For the transient sediment calculation routine, sediment continuity is written
for each time step. All numbers are in cubic meters.

Sedim. continuity: In, Out, DcDt, Bed, Move, ContDef., MoveDef:
Dt:  0.453509 20.995623 -20.666748 0.355497 0.110065 0.230863 0.245432
Sum: 0.888430 50.468110 16.613033 - 66.460044 -68.192414 -0.267331 1.732371

The first line gives the names of the variables in the two lines below. The
second lines give data for each time step, while the third line gives data for
accumulated time.

The first number is the inflow of sediments. The second is the outflow of
sediments. The third is the accumulated sediments in the water body. The fourth
is the calculated bed changes. The fifth is the actual bed changes. The sixth
is the continuity defect, and the second is the defect because of the bed
changes. The last two numbers should be small compared with the total flux in
the geometry.


ΓòÉΓòÉΓòÉ 4.3. The koordina and koomin files ΓòÉΓòÉΓòÉ

 The koordina file describes the bed of the geometry. An example is show in the
figure below. The grid can be made using a map, a spreadsheet or the Grid
Editor

Grid with numbering of lines and cells

The necessary input data is the x,y and z coordinates of the points where the
grid lines meet. The format of the data is given below.

i  j   x   y    z

An example

1  1  0.34  0.54  0.11
1  2  0.35  0.66  0.12

The first two numbers are integers, while the following three are floats. The
numbers are read in a free format, which means that the distance between them
does not matter. The sequence of the points are not important, as long as all
points are included. This is not controlled by the model, so the user must do
this by looking at the grid in the graphic modules of the program.

If a tunnel is simulated, or the user wants to specify the water surface, an
additional floating point number is read for each line. This gives the top
level for each grid intersection. An example:

1  1  0.34  0.54  0.11  1.21
1  2  0.35  0.66  0.12  1.33

To make SSIIM read the last float, the K 1 data set in the control file must
be: K 1 0 0

Some words about indexing and numbering of grid lines and cells. The variable
names for the number of grid lines in the three directions are:

xnumber : number of cross-sections
ynumber : number of longitudinal lines
znumber : number of horizontal lines

The numbering of the grid lines goes from 1 to xnumber in the streamwise
direction, and similarly for the other two directions.

However, the grid lines define cells between the grid lines. The variables are
calculated in the center of each cell. This means that a numbering for cells
also is required. The word node is often used for the center of a cell.

From a geometrical view of the grid, it is observed that the number of lines
always exceeds the number of cells by one in each direction. When the arrays
are defined, it is therefore a choice for the programmer to start the numbering
of the cells on one or two. The choice that is made in this program is that the
numbering starts on two. This means that the cell that is defined by grid lines
i=1 and i=2 and j=1 and j=2 has the number (2,2). Cell number (1,1) does not
exist. The numbering of the cells is also shown in Fig. 1. The numbering of the
grid lines is shown with the <,> sign, while the numbering of the calculation
nodes is shown with the (,) sign. The grid is non-staggered.

If SSIIM terminates and the boogie file contains the following message: Error,
negative areas for cell i=13, j=2, or some other combinations of i and j, then
there is an error in the koordina file. The indexes denote the cell number, so
for i=13, j=2, the x and y coordinates for the following grid line
intersections should be checked: (13,2); (13,1); (12,2) and (12,1).

The data on the koordina file defines a surface. It is possible to make a file
with exactly the same format and call it koomin. This surface is then used as a
minimum elevation surface for bed changes. The bed will not be lowered under
this surface.


ΓòÉΓòÉΓòÉ 4.4. The geodata file ΓòÉΓòÉΓòÉ

This file contains a number of x,y and z coordinates. An example is shown
below:

E 2.2 3.3 3.4
E 4.5 3.3 2.2
E 3.3 4.2 1.2

 The purpose of this file is to use geometrical data that has been obtained
from the field, a digitized map or a GIS system. These data would normally not
fit into a grid like the koordina file.

The file is used in three modules in the program. The first module is the
GridEditor, which can display the points in the file with the grid. This makes
it easier to generate the grid. The Utility option of the menu and the Show
geometrical points option in the pull- down menu activates this. The grid
points are displayed with different colors according to which level they are.

The second use for this file is also in the GridEditor. It is then used in the
Make bed interpolations for generating the z values for the bed of the grid. A
linear interpolation procedure is used.

The third use is to make the Porosity file. The module that does this is
activated from the main menu of the user interface, from File and Make porosity
file in the pull-down menu.


ΓòÉΓòÉΓòÉ 4.5. The bedrough file ΓòÉΓòÉΓòÉ

 This file is used to give a roughness height to individual bed cells.  Values
in this file overrides the value calculated from Manning's coefficient, and the
value given on the F 16 data set. On each line a character, two integer and a
float are given. The first character is a B, and the two following integers are
indexes for the bed cell. The float is the roughness in meters. An example is
given below:

B          19      2    0.001
B          19      3    0.001
B          19      4    0.001


ΓòÉΓòÉΓòÉ 4.6. The porosity file ΓòÉΓòÉΓòÉ

 Note: When using the porosity file, use a P on the F 7 data set.

This file is used when the bed of the river is covered by stones, and a
porosity term is used in some of the cells. This file describes the location
and magnitude of the porosity in the geometry. An example is given below:

P 17 6 3.349774 3.399189 3.450101 3.499517 0.000000 0.700000 0.833333 1.000000
P 17 7 3.358273 3.413603 3.470610 3.525940 0.000000 0.653846 0.807692 1.000000
P 17 8 3.403323 3.426084 3.449536 3.472297 0.000000 0.642857 0.785714 1.000000

 First, the character P is read. Then two indexes for the i and j number of the
bed cell is read. Then four vertical levels are read, which have the same zero
reference as the koordina file. The porosities in each of these levels are then
read.

 The porosity file can be made from a koordina file and a geodata file. The
module that does this is activated from the main menu of the user interface,
from File and Make porosity file in the pull-down menu. The procedure goes
through each element and used the points in the geodata file to obtain the
data.


ΓòÉΓòÉΓòÉ 4.7. The innflow file ΓòÉΓòÉΓòÉ

 This file is used to read velocities in three directions for the upstream
boundary condition. The program searches for this file, and uses the data on
the file if it exists. If the file does not exist, a warning message is written
to the boogie file, and the program proceeds normally.

 On each line the velocities in a cell of the upstream cross-section are given.
First, the character E is written. Then the indexes j and k (horizontal and
vertical) are given. Then the velocity components in the x,y and z directions
are given. An example is given below:

E  2  2  0.299115  0.023009  0
E  2  3  1.79469  0.138055  0
E  2  4  1.9941  0.153394   0
E  2  5  2.19351  0.168733  0

 The file does not have to contain values for all the nodes. The normal
initialization procedures are applied first, and then the innflow file is read.
The nodes that are not present in the innflow file will keep the values from
before the file was read.


ΓòÉΓòÉΓòÉ 4.8. The loggfil file ΓòÉΓòÉΓòÉ

 This is a file that is used to log bed changes between each time the bed is
changed. The bed changes are written with the "append" mode in C, so that for
the file to be updated, it must exist before SSIIM writes to it. What is
written to the file will be appended to what is present in the file.

 What is written to the file is a time step for each change, together with the
bed changes for each cell in meters. The bed sediment grain size distribution
for each time step is also written to this file.

 When SSIIM starts, it looks for a file called loggfil.pre, and if it exist, it
uses this file to change the bed and give initial bed sediment grain size
distribution. If one decides to start from a previous time step, one must have
copied loggfil to loggfil.pre before starting SSIIM.

 loggfil is written from the Bedchange+ option in the Map graphics module.

 The loggfil file is never overwritten by the program. New bed changes are
appended to the end of the file. The user must therefore take care so that only
the relevant data exist in the loggfil and loggfil.pre files.

 Note that if the program does not find the loggfil.pre file, a warning is
written to the boogie file, and the program proceeds normally.


ΓòÉΓòÉΓòÉ 4.9. The result file ΓòÉΓòÉΓòÉ

 This file contains the results from the water flow calculations. The file is
written when the prescribed number of iterations have been calculated or when
the solution has converged. The results are velocities in three dimensions, k,
Γûá, pressure, and the fluxes on all the walls of the cells. The data from this
file is used as input for the sediment flow calculations. This file can also be
read when the user wants to start the water flow calculations from where the
result file was last written (hot start).

 An example of a result file:

Results from SSIIM - flow, iter = 12910
Residuals: 0.000732 0.000588 0.000002 0.000003 0.001000 0.000000
Roughness : 0.050000
C 54 9 11
 i  j  k   u   v   w   k  e  f1  f2  f3  p
D  1  1  1 0.00000000e+00 0.00000000e+00 0.00000000e+00 0.00000000e+00 0.00000000e+00 0.00000000e+00 0.00000000e+00 0.00000000e+00 0.00000000e+00
D  1  1  2 0.00000000e+00 0.00000000e+00 0.00000000e+00 0.00000000e+00 0.00000000e+00 0.00000000e+00 0.00000000e+00 0.00000000e+00 0.00000000e+00
D  1  1  3 0.00000000e+00 0.00000000e+00 0.00000000e+00 0.00000000e+00 0.00000000e+00 0.00000000e+00 0.00000000e+00 0.00000000e+00 0.00000000e+00

D  2  4  7 6.31143968e-01 2.02894592e-01 -6.80367016e-05 6.47305125e-03 3.85539263e-04 3.47858729e+03 -5.19507052e+02 1.39776552e+03 1.91355310e+02
D  2  4  8 6.38189711e-01 2.05198514e-01 -2.09522025e-04 6.40727451e-03 3.13804122e-04 3.54203761e+03 -5.25291012e+02 1.09548199e+03 1.91350056e+02
D  2  4  9 6.42687814e-01 2.06670571e-01 -3.70305526e-04 6.37079494e-03 2.71714390e-04 3.58421958e+03 -5.28978103e+02 7.51732364e+02 1.91343817e+02

The first lines gives the residuals, the roughness and the grid size. Then each
line gives the nine values for one cell. The letter D starts the line, then the
three indexes for the cell. Then the three velocities, the k and epsilon
values. Then the fluxes in the three directions and finally the pressure. All
the parameters are placed on one line in the file.

All the results are given in SI units, so that for example the velocities are
in meters/second and the pressure is in Pascal, or Newton/m2.


ΓòÉΓòÉΓòÉ 4.10. The conres file ΓòÉΓòÉΓòÉ

 This file is written after the sediment concentration calculation has
finished. Each line in the file contains first three indexes indicating for the
node number. Then the total concentration is written and then lnumber floats
that give the concentration for the sizes. An example is given below:

1 1 21 0.000000e+00 0.000000e+00 0.000000e+00 0.000000e+00 0.000000e+00
1 2 2 5.075079e-04 0.000000e+00 1.026459e-04 1.030081e-04 1.032351e-04
1 2 3 4.064470e-04 0.000000e+00 1.011788e-04 1.015358e-04 1.017596e-04
1 2 4 4.004061e-04 0.000000e+00 9.967497e-05 1.000267e-04 1.002471e-04

 If a file conres.pre exist, this will be read by the program before the
sediment calculation starts. The conres.pre file has the same format as the
conres file.


ΓòÉΓòÉΓòÉ 4.11. The interpol and interres files ΓòÉΓòÉΓòÉ

 Vertical profiles of velocity or concentration are sometimes needed.
Coordinates for the locations where the profiles are wanted are given in this
file. When the write results routine is activated and the integer on the F 48
data set in the control file is above 1, it will search for this file. If this
file is not found, it will proceed normally and write the result or the conres
file. If the interpol file is found and the integer on the F 48 data set is
above 1, the program will not write to the result file, but write the
interpolated vertical velocities to a file named interres. An example of an
interpol file is given below:

M      2.03    0.5
M       4.06   0.39
M       4.06    0.5

 The character M is read first, and then the x and y coordinates for the point
one wishes to interpolate the vertical profile to. If the value on the F 48
data set is 3 the concentrations are interpolated. If the value on the F 48
data set is 2, the velocities, k and epsilon are written to the file. If the
value on the F 48 data set is 1, the bed levels are written (no profile, only
one point). The results are written to a file called interres.

An example of an interres file is given below:

C 9.250000 0.100000, size = 0
1.530130 0.000000e+00
1.491877 5.266262e-05
1.415370 9.303652e-05
1.338864 1.349549e-04
1.262357 1.740915e-04
1.185851 2.075269e-04

 The first line starts with a C, and then the x and y coordinates of the
vertical profile is given. Two columns follow. The first column is the z value
of the vertical profile. The second column is the concentration. If velocities
are interpolated instead of concentrations, an M is written on the first line
instead of the C. Instead of the concentration column, five calamus are
written. The variables in the columns are: velocity in x,y and z directions, k
and epsilon.

Note that the procedure for writing the interres file changed from SSIIM
version 1.3 to version 1.4.


ΓòÉΓòÉΓòÉ 4.12. The verify file ΓòÉΓòÉΓòÉ

 This file is used as input for the VerifyProfile graphics option. The user can
present calculated velocity or concentration profiles together with measured
values. Up to 20 vertical profiles in a section of the geometry can be shown.
The horizontal location of the profiles are determined by the user, so this
method of presentation can be used for both cross-sections, longitudinal
section or other user-defined sections. An example of a verify file is shown
below:

P 40.0 10.0 3
5.0 0.5 0.1
6.5 0.6 0.12
7.0 0.8 0.05
P 70.0 10.0 2
6.0 1.0 0.1
8.0 1.5 0.8

 Each profile is identified with a capital P. Then the x and y coordinates of
the point follow. The coordinates are given in the same system as the grid, or
the koordina file. After the coordinates, an integer is read. The integer tells
how many points are measured in this profile. Up to 11 points can be given. On
the following lines the data is given. There must be the same number of lines
as the integer on the P line. Three floats are given on each line. The first is
the vertical coordinate where the data is taken. This is given in the same
coordinate system as the grid, or the koordina file. The following two floats
are velocities or concentrations, depending on what is calculated. If
velocities are calculated, the second float is the velocity component in the
x-direction and the third float is the velocity in the y-direction. If
concentration is calculated, the second float is the measured concentration and
the third float is a dummy number which is not used. If concentrations are
given, the user can choose in the graphics presentation wheter a total
concentration or a fractional concentration is presented.

The example above gives two profiles. The first is located at x = 40.0 meters
and y = 10.0 meters. Three data points have been measured. The first point is
located at global coordinate z = 5.0 meters, and have a measured x-component
velocity of 0.5 m/s and a y- component velocify of 0.1 m/s. The second point is
located at global coordinate z = 6.5 meters, and have a measured x-component
velocity of 0.6 m/s and a y-component velocity value of 0.12 m/s.

Note that this file changed from SSIIM version 1.3 to version 1.4.


ΓòÉΓòÉΓòÉ 4.13. The timei and timeo files ΓòÉΓòÉΓòÉ

 There are two files that are relevant to time series calculations. The first
file, timei, is an input file for time series of discharge, waterlevel,
sediment concentration and control for output. The second file, timeo, is an
output file with time series from the model.

The timei file reads two types of data sets. The first type controls the output
to the timeo file. This data set begins with a capital O, and then reads a
float, Time, and an integer, Vars. Time is the time for when the print out
starts, and Vars tells how many variables are written to the timeo file for
each time step. Maximum 25 variables can be written. A maximum of 20 control
output data sets can be used.

After reading Time and Vars, the next lines read which variables are printed
and in which cell. Vars lines are read. Each line starts with a lowercase
character, and then three integers (four in case of sediment concentration) are
read. The integers indicate which cell the variable is located in. If sediment
concentration is read, the last integer tells which fraction is written. 0
indicates the sum of the fractions. The characters corresponding to different
variables are listed below:

character:  variable:
u      velocity in x-direction
v      velocity in y-direction
w      vertical velocity
p      pressure
k      turb. kin. energy
e      epsilon
d      turb. diffusion
z      vertical grid elevation
c      concentration

The second type of data set is input data. The line starts with a capital I,
and then five floats are read. The first float indicates the time for when the
following variables are used. The second float is the upstream water discharge.
The third float is the downstream water discharge. The fourth float is the
upstream water level, and the fifth float is the downstream water level.
Sometimes one of the last variables are unknown, and then a negative value can
be inserted and the program will try to calculate the value.

If the TFS method is used, lnumber floats are read additionally, indicating the
upstream inflowing sediment transport.

An example of a timei file is given below:

O 0.0 6
u 2 2 2
c 2 2 2 0
p 2 2 2
z 41 3 6
z 1 2 1
z 2 2 1
I 0.0 10.0 10.0 -20.0 19.5.0 0.000
I 100.0 10.0 10.0 -20.0 19.0 0.000
I 200.0 10.0 10.0 -20.0 18.5 0.000
I 300.0 10.0 10.0 -20.0 18.0 0.000
I 400.0 10.0 10.0 -20.0 17.5 0.000

 The timeo file gives the output time series from the calculation. For each
time step, a line of variables are written to the file. Each line has Vars
floats, according to which variables were given in the timei file. In the above
file six variables are written. The first variable is the velocity in
x-direction for cell (2,2,2). The second variable is the sum of all sizes of
concentration for cell (2,2,2). The pressure and vertical grid elevations for
various grid intersections are written.

The second group of parameters in the timei file is an input time series. Each
time step in the series are given on one line. The line starts with a capital
I. Then the time step is given. Then four floats are read. This is the upstream
and downstream water discharge and upstream and downstream water level,
respectively. If a negative value is given, the program will try to calculate
the value. The last float(s) are sediment concentration(s) for the various
sediment sizes. These are only read if the transient sediment calculation is
used. Note that the time steps does not have to correspond to the time steps of
the program. The sum of the calculated time steps is calculated by the program
and compared with the time step in the file. If the calculated time exceeds the
time from the file, the values from this data line will be used. The times must
be in increasing order.

An example of a timeo file corresponding to the above timei file is given
below:

0.0000e+00
2.0000e+00 8.804354e-01 6.837692e-04 -1.853305e+01 1.950000e+01 1.792479e+01
4.0000e+00 9.185002e-01 7.081983e-04 -3.949717e+01 1.950000e+01 1.792458e+01
6.0000e+00 1.100297e+00 1.121773e-03 5.289925e+01 1.950000e+01 1.792421e+01
8.0000e+00 1.156041e+00 1.389383e-03 8.122703e+01 1.950000e+01 1.792374e+01
1.0000e+01 1.207883e+00 1.614782e-03 9.418469e+01 1.950000e+01 1.792317e+01

Each line corresponds to a time step. A time step of 2 seconds have been used.
The first float is the calculated time. The second float is the velocity in
cell (2,2,2). Then the sum of the concentrations in cell (2,2,2) is written.
Then the pressure and the vertical grid elevations.

This format is chosen so that it is easy to import the file to a spreadsheet
for presentation.


ΓòÉΓòÉΓòÉ 4.14. The forcelog file ΓòÉΓòÉΓòÉ

 This file contains time series of the forces on one or more obstacles for the
transient free surface calculation. One line is written for each time step. An
example of a forcelog file is shown below:

Forces on block 1 : 271.062, 0.099838 N in x and y direction
Forces on block 1 : 398.574, 0.082644 N in x and y direction


ΓòÉΓòÉΓòÉ 4.15. The xcyc and koosurf files ΓòÉΓòÉΓòÉ

 The two files xcyc and koosurf contain the geometry of the grid. This is used
when restarting calculations which have changed the grid.

The koosurf file is identical to the koordina file, except that the surface
level is also written for each line. This is similar to using the koordina file
with the tunnel option.

The xcyc file contains the x, y and z values of all the grid intersections.

When writing the files from the menu, both files will be written. When reading
the files, SSIIM will try to read both files, but if the xcyc file is missing,
it will only read the koosurf file. The internal grid nodes will be generated
by linear interpolation, as given on the G 3 data set in the control file.

If the internal nodes of the grid are generated by linear interpolation, the
only necessary file is the koordina file. However, for calculations where some
part of the grid moves, and some is outblocked and does not move, it is
necessary to save the xcyc file, and let SSIIM read this.


ΓòÉΓòÉΓòÉ 5. Advice for users ΓòÉΓòÉΓòÉ


ΓòÉΓòÉΓòÉ 5.1. Advice for new users ΓòÉΓòÉΓòÉ

 Generally, it is advisable to start with reading this manual. It is important
to understand that the model is made up of several sub-models. This is
reflected in the different choices in the main menu which is used to start the
sub-models. Some models can be run simultaneously.

The hardware requirements for running the program are mainly focused on having
enough RAM. In the beginning of the boogie file it is printed how much RAM the
program allocates for the arrays. This can be added to the RAM requirement for
the program itself, about 1.2 MB, plus what the operating system requires. An
estimate for the amount of RAM is thereby obtained. OS/2 will use the harddisk
as extra memory if there are not sufficient RAM. The penalty is that the
program runs very much slower. This situation can be detected by observing if
the system swaps to the harddisk while running only the SSIIM program. The
water flow module may take from some hours to some days to converge for a
typical case, when there is enough RAM. However, under OS/2 it is not any
problem to let the program run in the background while doing other tasks on the
computer.

 An advice for the first-time user is to run the tutorial and one of the
example cases. Try to modify some of the parameters and run it again. Often the
user wants to simulate a particular case. It is then advisable to try to find a
similar example case and modify this step by step.

Some words about crashing the program and input control. There are various
controls for input and checking of intermediate results. If any of these
controls finds something wrong, an error message is written to the boogie file,
and the program may terminate. Therefore, if the program suddenly stops, and
the main user interface disappears, check the boogie file for possible error
messages.

Two files are required to run the program. These are called koordina and
control. The koordina file contain the grid. The control file contain the rest
of the necessary parameters. The newer versions have new options for making the
input data for the control file, and there is also a Grid Editor that can be
used to make the koordina file.

 Finally, the results from the program ought to interpreted according to:

- Possibilities of bugs in the program making errors
- Previous cases where the results have been compared with measurements
- Numerical errors, like false diffusion, grid independence, etc.
- Accuracy of boundary conditions

Knowledge and experience in computational fluid dynamics and hydraulic
engineering are essential for the assessment of the validity and accuracy of
the results. Also see advice for interpretation of results.


ΓòÉΓòÉΓòÉ 5.2. The grid ΓòÉΓòÉΓòÉ

 Making the grid is often the most time-consuming process in the preparation of
input data for SSIIM. The general idea is to divide the water body into cells.
The size and alignment of the cells will strongly influence the accuracy of the
calculation, the convergence and the computational time.

The grid used in SSIIM is structured. This can make it difficult to adapt the
grid to complex geometries without loss of accuracy or slow convergence. In the
following there are given some guidelines of how to make a good grid. Also, it
is recommended to read Chapter 4.4 first, to understand the index system of the
grid lines.

If the water body is rectangular, it is possible to use a spreadsheet to make
the grid. However, in most cases, the fastest way to make the grid is to use
the GridEditor. It is recommended to read Chapter 3.3 and try the tutorials to
get to know the GridEditor.

When the grid is made, a backwater calculation is carried out to determine the
initial water surface. The water surface will therefore have a downward slope
from cross-section j=1 to cross-section j=ynumber. The parameter ynumber is the
number of cross-sections. Also, by default, the given discharge is flowing into
cross-section j=1 and out of cross- section j=ynumber. Therefore, when making
the grid, be sure that the line j=1 is the upstream cross-section of the
geometry, where most of the water enter the geometry.

Here is some advice on how to shape the cells:

1 Make the grid line intersections as perpendicular as possible. It is not
adviceable to have intersections with an angle of less than 45 degrees. Non-
orthogonality in the grid will make the convergence slower. It is recommended
to use the elliptic grid generator to make the grid smoother.

2 Try to align the grid lines in the streamwise direction paralell to the
velocity vectors. This will decrease false diffusion.

3 The distortion ratio should not be too great. The distortion ratio is the
dimension of the grid in one direction divided by the dimension in another
direction. Some people say this should be less than 2 (two), but other people
have obtained good results for ratios up to 10. On occations, ratios of up to
100 have been used. This gave reasonable results, but it required very low
relaxation coefficients and an extremely large number of iterations to
converge.

4 The size of a grid cell should not be too much larger than its neigbours.
Some people say the increase in size should not be greater than 20 %. On some
occations this value have been over 1000 % (a factor 10). Some of these cases
gave reasonable results, but other cases gave unphysical results. A
recommendation is to try to stay within 50 %, but if much larger values are
used, be aware that unphysical results may occur. Unphysical results can be
velocity vectors that point in another direction than what seems natural, for
example not paralell to walls.

 The following two chapters give more advice on convergence and interpretation
of the results:

Experience with convergence for the water flow calculation

Advice for interpretation of results


ΓòÉΓòÉΓòÉ 5.3. Experience with convergence and crashes ΓòÉΓòÉΓòÉ

 There are three ways SSIIM can crash:

1.   The program stops calculation and the dialog box says there is an error.

2.   The program stops and exits, the menu and the dialog box disappear.

3.   The program stops with an OS/2 system error, usually floating point
invalid    operation, overflow or underflow error.

Often an error message is written to the  boogie  file before the crash occur.
This happens particularly for type 1 and 2 of this list above. If an error in
the input files are detected, an error message is written to the boogie file
and type 2 crash occurs. If the program crashes, it is therefore recommended to
take a look at the boogie file. If crash type 1 occurs, it is also possible to
look at the graphics to try to see where in the geometry the problem is.

If the boogie file contains the following message: Error, negative areas for
cell i=13, j=2, or some other combinations of i and j, then there is an error
in the koordina file. The indexes denote the cell number, so for i=13, j=2, the
x and y coordinates for the following grid line intersections should be
checked: (13,2); (13,1); (12,2) amd (12,1).  Crashes during initiation of the
water surface  The initial water surface calculation is a 1 D backwater
calculation using Manning's formula for the friction loss. When this does not
converge the program may crashes with no error messages, except an OS/2 error
message that tells that the program had caused a floating point overflow error.
This usually happens when there is supercritical flow somewhere in the
geometry. The remedy is twofold:

 1. Increase the number of cross-sections for the initiation on the W 2 data
set in the control file.

2. Choose higher Manning's friction factors on the W 1 or the W 5 data set in
the control file.

 This procedure has so far worked for all the cases where this problem has
occurred.

 Crashes with underflow error  For some cases the program can crash with an
underflow error (type 3 crash). This happens particularly when some part of the
geometry is blocked out. The reason is that a variable is multiplied with
10e-30 for each outblocked cell, and when the solver multiplies these together
and there are sufficient outblocked cells to get below 10e-300 an underflow
exception occurs. To prevent this there has to be an if-statement inside the
solver loop, and this slows down execution of the program slightly. Therfore
two solvers are incorporated, and if the F 43 data set is used, the solver with
control of underflow error is used. Calculations with default values of F 43
will not check for underflow errors.  Convergence  There are four main
calculation algorithms in SSIIM:

1. Initial water surface calculation
2. 3D water flow field
3. 3D sediment flow field
4. Water quality

The sediment calculation has always converged, although sometimes it may take
some time. Presently, it is believed that the water quality calculation also
will not experience major convergence problems.  The main problem is then to
get the 3D water flow field calculation to converge. Generally, in
computational fluid mechanics cases it is often a problem to get the solution
to converge. Two factors are important:

 - A good grid.
 - Proper relaxation coefficients.

It is presumed that the boundary conditions are correct, which is always a good
thing to check in case of low convergence or strange results.

 Experience shows that the degree of non-orthogonality of the grid will affect
the convergence. A higher degree of non-orthogonality will give slower
convergence. A slower convergence will also be experienced where strong
gradients are present. This applies for example at the inflow of a jet from a
wall.

 For the convergence of the k and epsilon equations for river problems, the
size of the cell closest to the bed is important. This can be changed by
changing the second number in the G 3 data set in the control file. This
parameter also depends on the roughness of the bed. The size of the bed cell
should increase with increasing roughness. The height of the bed cell should
not bee too much smaller than the roughness of the bed.

The default values of the relaxation coefficients are set to 0.8 for the
velocity equations and 0.2 for the pressure-correction equation. For k and
epsilon, 0.5 is used as default. The values of the relaxation coefficients for
the velocity equations and the pressure-correction equations are presumed to
give an optimum convergence for the average flow case. Values of 0.5 for all
equations will often give a slower convergence, but with less probability of
divergence. Theoretically, the sum of the relaxation coefficient for the
velocity equations and the relaxation coefficient for the pressure-correction
equation should be unity for optimum convergence. However, for some difficult
cases this rule has to be abandoned.

 If the solution blows up after the first few iterations, it is possible to set
the relaxation coefficients very low, and then increase the coefficients for
the following iterations.

 For some cases where the equation for k is slowest in convergence, a more
rapid convergence has been achieved when changing the relaxation coefficient
for k from 0.5 to 1.0 after several iterations.

 For many cases it can be said that lower relaxation coefficients will give
less instabilities during the convergence, but a slower convergence. Higher
relaxation coefficients will give more rapid convergence if there are no
instabilities. This is however only a rule of thumb, which does not apply to
all cases. Instabilities can be observed during the iterations when the
residual or the velocities increase and decrease periodically.

 Use of block-correction will lead to a more rapid convergence. There is
however a possibility of this procedure leading to negative values of k. The
program will then crash because in the wall laws the square root of k is
calculated. The multi-block flow module avoids this problem never using a k
value below 10-9. This value is equivalent bed shear stress of 3.0x10-7 N/m2,
and an interpretation of this minimum value is that the bed shear stress also
has a minimum value of 3.0x10-7 N/m2.

 For some cases there have been problems getting the solution to converge if
there are parts of the geometry that has relatively low total velocity.
Experience has shown that the initial conditions then may be important. If such
a situation is present it is important to start the iterations with very low
initial velocities. This is done with the G 8 data sets.

 Transient calculations

If during steady calculations there are oscillations in the velocities, this
may be a sign that the flow field has a transient charachter. One may then
invoke the transient calculation and a periodical transient solution may be
observed. However, another possibility is that the oscillations disappear after
adding transient terms. The transient terms can have a stabilizing effect on
the solution.

 Note that a non-transient solution may very well emerge even though the
corresponding prototype flow field has transient oscillations.

 Transient free surface calculations

 The transient free surface algorithm is somewhat unstable. A remedy to cause
more stability is to increase the number of inner iteration pr. time step.
Perhaps a better method is to decrease the time step. If the changes in water
surface with time are very small, it is recommended to use option 2 instead of
option 1 on the F 37 data set. This is a more stable algorithm.


ΓòÉΓòÉΓòÉ 5.4. Advice for interpretation of results ΓòÉΓòÉΓòÉ

 As mentioned earlier, it is advisable to have experience in computational
fluid dynamics when proper interpretation of the results is required. Some
guidance is given below.

 An important numerical effect that can deteriorate the results is false
diffusion. This effect is most noticed for first-order schemes, including the
POW scheme. The effect depends on how well the flow velocity vectors are
aligned with the grid lines. For small alignment angles, the effect is small.
Maximum false diffusion will happen when the grid lines are aligned 45 degrees
with the flow. The amount of false diffusion also depends on the size of the
grid cells.

 There are three methods to decrease the amount of false diffusion:

1. Decrease the size of the grid cells == increase the number of cells
2. Align the grid with the flow field
3. Use the second-order upwind scheme

Point 2 may be difficult in a practical situation. However, the calculations
should be carried out using approach 1 and/or 3 to assess the effect of false
diffusion.

 Another important aspect is the boundary condition. This especially applies to
the inflowing boundary. If the velocity field at the inflowing boundary is not
known exactly, one should try different velocity distributions to try to assess
the effect of this parameter. For a river running into a reservoir, it is
possible to model a part of the river upstream of the reservoir, and thereby
obtaining a better estimate for the velocity distribution where the river
enters the reservoir. The upstream boundary condition is also important for
sediment calculations, where both the total amount of sediment inflow and the
sediment grain size distribution can be varied. For the bed boundary, it is
possible to vary the roughness to investigate the effect of this parameter. It
can also sometimes be advantageous to make variations for the formula for
sediment concentration close to the bed. This especially applies for sediment
particles outside the range for which the formula is applied for.

 When interpreting the results from the model it is also important to keep the
accuracy of model in mind. The k-epsilon turbulence model has limitations in
how accurate the turbulence field is predicted. This will also affect the
velocity field. For example, when calculating the recirculation zone for a step
case, the length of the recirculation zone can often not be predicted with any
better accuracy than 10-30 %.

 In some situations the water flow will be time-dependent. An example can be
oscillations behind a cylinder or in an expansion. It is possible to obtain a
converged steady solution from the model although the physical problem is
unsteady. This must be considered when interpreting the results. The effects of
an unsteady solution compared to the given solution should be assessed if this
is probable. When an unsteady case is solved with a steady method there can be
convergence problems. If the relaxation factors have to be fairly low to get
the solution to converge, this can be an indication that the flow field may be
unsteady.

 Another topic of interpretation is the resolution of the calculated flow field
compared with the size of the grid cells. Several cells are required to
dissolve a recirculating zone. Flow field characteristics smaller than about
4-7 cells may not show up in the solution. And a recirculation zone with very
few cells may be inaccurately calculated because a certain resolution is
required.

 For some flow geometries the Navier-Stokes equations may have more than one
solution. This can for example be seen in a flume with a symmetric expanding
channel, where the jet may follow one side of the channel. If an obstacle is
inserted into the side with the jet, the jet moves to the other side of the
channel. This phenomena have also been experienced in non-symmetrical
expansions, when varying the number of grid cells caused the Navier- Stokes
equations to converge with a completely different flow field. It is thought
that this problem has a higher risk of occurance in geometries with expansions
and recirculation zones, and also if the Second-Order Upwind scheme is used
instead of the Power-Law Scheme.


ΓòÉΓòÉΓòÉ 6. Tutorial ΓòÉΓòÉΓòÉ

 This tutorial is meant for first time users of the SSIIM program. The tutorial
shows the main features of the user interface, with the presentation graphics,
animation and grid editing. The user is not required to edit files, but some
knowledge of grids is recommended. It is important to know the purpose of the
the control and koordina input files. During the tutorial the files will be
made interactively. The tutorial does not show the more advanced features of
the program, which necessitates editing of the input files.

 The tutorial is divided in four stages. During the first stage the two input
files are made. During the second stage the presentation graphics is shown. The
third stage familiarizes the user with the grid editor. The animation graphics
is shown in the fourth stage.


ΓòÉΓòÉΓòÉ 6.1. First stage ΓòÉΓòÉΓòÉ

 In this stage the two user input files control and koordina are made.

 Start up ssiim from a directory where the files control and koordina do not
exist. This is done by writing [path]ssiim13 <CR> when you are on this
directory. The [path] is here the path were the executable program for SSIIM is
placed.

 After this a dialog warning box shows up on the screen, telling you that the
control file is not found, and that you have to fill in the parameters in the
next dialog box. Choose OK in the warning box, and you see the main parameters
dialog box. Default values are present in the edit fields. Click on the edit
field for lines in streamwise direction. Change this value from 4 to 10 or a
higher value. Also change the number of lines in cross- streamwise direction
from 4 to for example 6. After this, push the OK button with the mouse. The
control file is then automatically made, and written to the disk.

 Immediately after this you will get a second warning box, which tells you that
the files koordina or geodata are not found. The file geodata can be used
initially instead of the koordina file, but that is a more advanced topic which
you can read more about after this tutorial. Push the OK button on the warning
box, and a new dialog box emerges. In this box you give the dimensions of the
grid. The default grid that is made initially is rectangular. You can choose a
grid which is 11 meters long and 6 meters wide. Change value in the editfields
from 10.0 to 11.0 for the length and from 5.0 to 6.0 for the width. Then push
the OK button. After this, the koordina file is made and written to the
harddisk. Immediately afterwards the normal user interface for the program is
shown and the program is started. The flow field for this grid is made in the
second stage


ΓòÉΓòÉΓòÉ 6.2. Second stage ΓòÉΓòÉΓòÉ

 In this stage we will solve the flow field for the given grid, and look at the
results.

 The main user interface is a dialog box and a menu bar. The dialog box will
show intermediate results from the calculations and other messages. The menu is
used for starting different sub-modules of the SSIIM program.

 In the first dialog box to make the control file, we gave a Manning's
coefficient, water discharge, downstream waterlevel and dimension of the
geometry. This is all we need to calculate the flow field with the
Navier-Stokes equations. To start the solution of the Navier-Stokes equations
you select the option Computations from the main menu. Then select MB-Flow from
the pull-down menu. After this, push the update button on the dialog box to see
how the residuals develop. The dialog box shows the residual for all the six
partial differential equations that is solved for the water flow calculation.
The water flow calculation is converged when all the residuals are under 0.001.

After convergence, we want to see the results. Choose the Graphics option of
the main menu, and the Map option in the pull-down menu. This gives you a
graphics view of the grid as seen from above. Choose Graph from the menu in the
map window, and Velocity from the pull-down menu. Then you see the velocity
vectors. You can scale and move the plot by using the <Page up>, <Page down>
and arrow keys. You can also scale the velocity vectors by choosing Scale and
VarEnlarge/VarShrink. And you can see the other parameters than the velocity by
choosing different variables in the Graph pull-down menu.

The velocity vectors are not too exciting for this channel and to make a more
complex flow pattern, you need to change the grid. This is done in the third
stage.


ΓòÉΓòÉΓòÉ 6.3. Third stage ΓòÉΓòÉΓòÉ

 In this stage we will concentrate about the grid editor. But first, we want to
show several graphic windows on the same time on the screen. Therefore, use the
mouse and push the main menu down in the lower left quadrant of your screen.
Scale the map window so that it fits in your upper left quadrant of the screen.
To fit the grid in the window, choose the Scale option in the map window and
Shrink in the pull-down menu together with the Move option in the map window
and left, down options in the pull-down menu.

 Then start the grid editor by choosing Input Edit from the main menu bar and
GridEdit from the pull-down menu. Scale and move the window and the grid so
that it fits in your upper quadrant of your screen.

 To edit the grid, you first choose some points which will not be affected by
the interpolation routines. This is done in a special modus of the editor. This
modus is invoked by choosing Define from the menu and Set NoMovePoints from the
pull-down menu. To verify that this modus is chosen, the letters "Point mode,
0" is shown on the lower part of the editwindow. The integer shows how many
points you have chosen. We want to choose four points, all on the upper
boundary of the grid. A point is chosen by clicking with the mouse on a grid
intersection. If successful, a blue star emerges at the grid intersection. For
a further explanation on which points to choose, see Fig. A. After choosing the
points we return to normal modus. This is done by choosing Define and Set
NoMovePoint again. We observe that this modus disappears because the text
"Point mode, 4" disappears.

Now we want to move the points. You can move any of the grid intersections by
clicking on the intersection with the mouse and dragging it to another place
and then release the mouse button. Try this with one of the intersections
between the marked points. In the following the four marked points are denoted
1,2,3 and 4, starting from left. Move point 2 and 3 down midway into the
channel. The grid should look like Fig. B afterwards. Then choose Generate from
the menu and Boundary from the pull-down menu. This makes straight lines at the
boundary. The grid will look like Fig. C. Now you see why we had to make the
"NoMovePoints". Then choose Generate from the menu and Elliptic from the
pull-down menu. Do this a couple of times until the grid looks ok. Now you have
generated an elliptic grid, which looks something like Fig. D.

 Next, we want to calculate the flow field for this grid. To increase the
visual effect, first go to the map window in the left upper corner, and start
the timer with 5 seconds interval. This makes the map window and the results
dialog box refresh automatically every 5 seconds. The timer is started by first
choosing Timer in the map window, and choosing 5 S on the pull-down menu. Then
choose Timer once more, but this time choose Start from the pull-down menu. You
can observe that the window is refreshed every 5 seconds.

 To apply the changes from the grid editor, go back to the grid editor window
in the upper right quadrant, and choose Utilities from the menu and  apply
changes from the pull-down menu. Then restart the water flow calculation by
choosing Computations from the main menu and MB-Flow from the pull-down menu.
Watch the results in the map window and the residuals as the solution
converges.

In the fourth stage we look at particle animation.


ΓòÉΓòÉΓòÉ 6.4. Fourth stage ΓòÉΓòÉΓòÉ

 In this stage we look at the animation. This is started by choosing Graphics
from the main menu and Animation from the pull-down menu.

When the window opens, a cross is displayed in the center of the window. Click
with the mouse on the center of the cross. This scales the mouse location for
the particle movement.

The grid seen from above is then shown. Move and scale the window and the grid
so that it fits in the lower right quadrant of your screen. Click with the
mouse inside the grid at the upstream part. Watch the particle that moves to
the place you chose. Start the animation by choosing Particle in the menu and
run on the pull-down menu.

After a while, click with the mouse on another part of the grid, and watch what
happens.


ΓòÉΓòÉΓòÉ 7. Examples ΓòÉΓòÉΓòÉ

 Several example cases are presented. Some of the examples includes the input
files for the cases, including the control.xxx and the koordina.xxx file. The
files can be used for SSIIM calculations by removing the extensions of the
files.


ΓòÉΓòÉΓòÉ 7.1. X shaped channel crossing ΓòÉΓòÉΓòÉ

 The files have extensions .x. In this example two channels cross. The example
is used to test the multi-block flow routine. Two extra blocks are added to
create the geometry. The geometry is symmetric, so the result should also be
symmetric.  The grid, seen from above  Velocity vectors, seen from above, level
6  Contour map of horizontal velocity, level 6  Contour map of vertical
velocity, level 10


ΓòÉΓòÉΓòÉ 7.2. Y shaped channel ΓòÉΓòÉΓòÉ

 The files have extension .y. A channel branches in two at an angle of 45
degrees. The two branches have identical boundary geometry. The case was
initially thought of being used for symmetry testing. However, the grid is not
symmetrical, and therefore the flow field will not be completely symmetrical.
This case is instead used for demonstrating sediment transport.  Contour map of
horizontal velocity, bed level (level 2)


ΓòÉΓòÉΓòÉ 7.3. Curved channel ΓòÉΓòÉΓòÉ

 The files have extensions .svi. The channel is used for testing the programs
ability to calculate the secondary flow pattern in a curved channel. It is also
used for testing the routine that recalculates the water surface location based
on the 3D flow field. The cross- sectional slope corresponds very well to
theoretical solutions.  Grid of channel, seen from above  Contour map of
vertial velocity, level 6  OpenGL color map of depth. Blue is minimum value and
red is maximum value.  OpenGL color map of cross-secton at downstream end. The
velocity vectors are parallell to the plane. The colors show velocity normal to
the plane. Blue is minimum value and red is maximum value.


ΓòÉΓòÉΓòÉ 7.4. Fish farm tank ΓòÉΓòÉΓòÉ

 The files have extensions .kar. This case is used for demonstrating inflow and
outflow at different locations in the geometry. The inflow is on one side, at
45 degrees to the wall. The outflow is at the bottom of the tank. The case is
also used for demonstration of fish habitat. It is also suited for particle
animation because the particle will move in a circular pattern. This case is
further described by Olsen and Alfredsen (1994).  Grid, seen from above
Velocity vectors at bed  Velocity vectors at level 10


ΓòÉΓòÉΓòÉ 7.5. Reservoir sedimentation ΓòÉΓòÉΓòÉ

 The files have extension .res. This case is used for demonstration of trap
efficiency calculation in a reservoir. It is a modified version of the Mae Tian
reservoir calculation case from Thailand (Olsen and Melaaen, 1993 a,b). 8.3
cubic meters of water is flowing in through the reservoir. Several sediment
sizes are used. The user can see the contour map of the bed levels, color map
of the bed level changes, cross-section velocities and longitudinal profiles of
the sediment concentration.  Grid, seen from above  Contour map of bed levels


ΓòÉΓòÉΓòÉ 7.6. 3D flood wave around building ΓòÉΓòÉΓòÉ

 The files have extension .wav. This example shows a flood wave in a 50 m long
and 25 meter wide channel hitting a square building with sides 5 meters. The
upstream water surface is 3 meters above the bed, and a water velocity of 3 m/s
is in the inflowing water. The speed and the depth of the wave correspond to
hydraulic formulas. The case is presented by Olsen (1994). Forces on the
building are written to the forcelog file. A verification study for this
example is presented by Lovoll et al (1995).  Velocity vector map, seen from
above, after 12 seconds

The following figures are longitudinal profiles along the centerline of the
geometry.  After 1 second After 5 seconds After 9 seconds


ΓòÉΓòÉΓòÉ 7.7. Sand trap ΓòÉΓòÉΓòÉ

 The sand trap case is a verification case, where an 18 m long physical model
of a sand trap were studied. The with of the sand trap was 1 m and it had a
height of 1.5 m. The results from the physical model study compared fairly well
with the results from the numerical model. For a further description of this
study, see Olsen and Skoglund (1994) and Olsen and Chandrashekhar (1995).
Example input files are not provided.  Comparision of calculated (lines) and
measured (X) velocity profiles in a longitudial section, with a modified
turbulence model.  Comparision of calculated (lines) and measured (X)
concentration profiles in a longitudial section, with a modified turbulence
model.  Comparision of calculated (lines) and measured (X) velocity profiles in
a longitudial section, with the standard turbulence model.  Comparision of
calculated (lines) and measured (X) concentration profiles in a longitudial
section, with the standard turbulence model.


ΓòÉΓòÉΓòÉ 7.8. Time-dependent evolution of scour ΓòÉΓòÉΓòÉ

 The input files have extension .sco.

The example is scour in a channel caused by an object decreasing the
cross-section area of the channel. This would normally also cause local scour
around the object. However, to avvoid excessive computer calculation time, a
very coarce grid is used. This grid is not fine enough to resolve the current
around the obstacle which is causing the local scour. To get a more reliable
prediction of the scour depth, a finer grid has to be used.

The time step is chosen to be 1000 seconds. This is also to avvoid excessive
computation time when running the example. This allows the user to observe how
the bed evolution changes. The time step is however to long to give an accurate
prediction of the evolution of the scour.

Note the grid extends relatively far downsteam of the obstacle. For some cases
this has shown to be necessary to avvoid unphysical results at the downstream
boundary.

The development of the scour hole is best seen with the contour map graphics or
the OpenGL graphics, showing the bed level seen from above. Note some bugs in
the contour map graphics causes some lines not to be shown at all times.


ΓòÉΓòÉΓòÉ 7.9. Water quality with Streeter-Phelps model ΓòÉΓòÉΓòÉ

 The input files have extension .qua

The water quality in a river is modeled with the Streeter-Phelps model. This
has two water quality constitutents: Organic substance measured in Biological
Oxygen Demand (BOD) and Oxygen Saturation Deficit (OSD). The
convection-diffusion equation for each constituent is solved, including source
terms for biochemical reactions.

Start by calculating the water flow field using MB-Flow2D or MB-Flow3D.
Afterwards, start the water quality calculation. You may use the calculation
menu.

The OpenGL 2D graphics is well suited to show the results.

This case is used for testing the numerical model against an analythical
solution.


ΓòÉΓòÉΓòÉ 7.10. Example of unstructured grid SSIIM 2.0 ΓòÉΓòÉΓòÉ

 SSIIM version 2.0 is planned to have a more flexible grid, with multiple
blocks, creating an unstructured grid. One procedure to generate the grid can
be seen from the following figures.

The grid editor is similar to the previous versions in the respect that points
in the window from the geodata file is shown. Then the user can make several
blocks, like shown below. The sides of the grid is then connected.  Each block
is then adjusted according to the boundary.  In the resulting grid, the blocks
are connected.  A bed interpolation routine gives a varying number of grid
cells in the vertical, as shown in the longitudinal profile below.  Another
procedure is to use a paving algorithm. This is shown on the figures below,
generating an unstructured mesh for a circular geometry


ΓòÉΓòÉΓòÉ 8. Literature ΓòÉΓòÉΓòÉ

 Ackers, P. and White, R. W. (1973) "Sediment Transport: New Approach and
Analysis", ASCE Journal of Hydraulic Engineering, Vol. 99, No. HY11.

Ashworth, R. (1993) "Renormalisation Group Turbulence Model", Eight
International Conference on Numerical Methods in Laminar and Turbulent Flow,
Swansea, UK.

Blacker, T. D. and Stephenson, M. B. (1991) "Paving: A new approach to
automated quadrilateral mesh generation", Int. Journal for Numerical Methods in
Engineering, Vol. 32, pp 811-847.

Brooks, H. N. (1963), discussion of "Boundary Shear Stresses in Curved
Trapezoidal Channels", by A. T. Ippen and P. A. Drinker, ASCE Journal of
Hydraulic Engineering, Vol. 89, No. HY3.

Chandrashekhar, J. (1994) "Numerical Simulation of Sediment Movement in
Desilting Basins using SSIIM", M.S. Thesis, Division of Hydraulic and
Environmental Engineering, The Norwegian Institute of Technology, Trondheim.

Einstein, H. A. and Ning Chien (1955) "Effects of heavy sediment concentration
near the bed on velocity and sediment distribution", UCLA - Berkeley, Institute
of Engineering Research.

Engelund, F. (1953) "On the Laminar and Turbulent Flows of Ground Water through
Homogeneous Sand", Transactions of the Danish Academy of Technical Sciences,
No. 3.

Engelund, F. and Hansen, E. (1967) "A monograph on sediment transport in
alluvial streams", Teknisk Forlag, Copenhagen, Denmark.

Kjellesvig, H. M. (1996) "Numerical modelling of flow over a spillway",
HYDROINFORMATICS-96, Zurich, Switzerland.

Kjellesvig, H. M. and StЫle, H. (1996) "Physical and numerical modeling of the
Himalaya Intake", 2nd Int. Conf. on Modelling, Testing and Monitoring for Hydro
Powerplants, Lausanne, Switzerland.

Lovoll, A., Lysne, D. K. and Olsen, N. R .B. (1995) "Three-dimensional modeling
of flood waves around a structure", Submitted to the 26th IAHR Biennial
Congress, London.

Lovoll, A. (1996) "Hydrodynamic forces from steep waves in rivers", Dr. Ing.
dissertation, Department of Hydraulic and Environmental Engineering, The
Norwegian University of Science and Technology.

Lysne, D. K., Olsen, N. R. B., StЫle, H and Jacobsen, T. (1995) "Withdrawal of
water from sediment carrying rivers. Recent developments in planning and
operation of headworks", International Journal on Hydropower and Dams, March.

Mayer-Peter, E. and Mueller, R. (1948) "Formulas for bed load transport",
Report on Second Meeting of International Association for Hydraulic Research,
Stockholm, Sweden.

Melaaen, M. C. (1992) "Calculation of fluid flows with staggered and
nonstaggered curvilinear nonorthogonal grids - the theory", Numerical Heat
Transfer, Part B, vol. 21, pp 1-19.

Olsen, N. R. B. (1991) "A numerical model for simulation of sediment movements
in water intakes", Dr. Ing. Dissertation, The Norwegian Institute of
Technology, Trondheim.

Olsen, N. R. B. and Melaaen, M. C. (1993) "Numerical Modeling of Erosion around
a Cylinder and Sediment Deposition in a Hydropower Reservoir", Eight
International Conference on Numerical Methods in Laminar and Turbulent Flow,
Swansea, UK.

Olsen, N. R. B. and Melaaen, M. C. (1993) "Three-dimensional numerical modeling
of scour around cylinders", ASCE Journal of Hydraulic Engineering, Vol. 119,
No. 9, September.

Olsen, N. R. B., Jimenez, O., LЫvoll, A. and Abrahamsen, L. (1994) "Calculation
of water and sediment flow in hydropower reservoirs", IAHR International
Conference on Modeling, Testing and Monitoring of Hydropower Plants, Hungary.
click here for graphics

Olsen, N. R. B. and Alfredsen, K. (1994) "A three-dimensional model for
calculation of hydraulic parameters for fish habitat", IAHR Conference on
Habitat Hydraulics, Trondheim, Norway.

Olsen, N. R. B. (1994) "SSIIM - A three-dimensional numerical model for
simulation of water and sediment flow", HYDROSOFT-94, Porto Carras, Greece.

Olsen, N. R. B. and Skoglund, M. (1994) "Three-dimensional modeling of water
and sediment flow in a sand trap", IAHR Journal of Hydraulic Research, No. 6,
Vol. 32.

Olsen, N. R. B. and Tesaker, E. (1995) "Numerical and physical modeling of a
turbidity current", 26th IAHR Biennial Congress, London.

Olsen, N. R. B. and Oldervik, O. (1995) "Three-dimensional numerical modeling
of water flow through a gate plug", 26th IAHR Biennial Congress, London.

Olsen, N. R. B. (1995) "Numerical modelling of hydropower reservoir flushing",
International Conference on Hydropower into the next Century", Barcelona,
Spain.

Olsen, N. R. B. and Stokseth, S. M. (1995) "Three-dimensional numerical
modeling of water flow in a river with large bed roughness", IAHR Journal of
Hydraulic Research, No. 4, Vol. 33.

Olsen, N. R. B. and Chandrashekhar, J. (1995) "Calculation of water and
sediment flow in desilting basins", 6th. International Symposium on River
Sedimentation, New Delhi, India.

Olsen, N. R. B. and Melaaen, M. C. (1996) "Three-dimensional numerial modeling
of transient turbulent flow around a circular cylinder", 2nd. Int. Conf. on
Modelling, Testing and Monitoring for Hydro Powerplants, Lausanne, Switzerland.

Olsen, N. R. B. (1996) "Three-dimensional numerical modelling of local scour",
HYDROINFORMATICS-96, Zurich, Switzerland.

Olsen, N. R. B. (1997) "Computational fluid dynamics as a tool for prediction
of sedimentation and erosion in reservoirs", Q. 74 a), ICOLD Conference,
Florence, Italy.

Patankar, S. V. (1980) "Numerical Heat Transfer and Fluid Flow", McGraw-Hill
Book Company, New York.

Rhie, C.-M, and Chow, W. L. (1983) "Numerical study of the turbulent flow past
an airfoil with trailing edge separation", AIAA Journal, Vol. 21, No. 11.

Van Rijn, L. C. (1987) "Mathematical modeling of morphological processes in the
case of suspended sediment transport", Ph.D Thesis, Delft University of
Technology.

Rodi, W. (1980) "Turbulence models and their application in hydraulics", IAHR
State-of- the-art paper.

Schlichting, H. (1979) "Boundary layer theory", McGraw-Hill.

Sintic, A. (1996) "Numerical models for dam-break flood routing", MS Thesis,
Institute of Hydraulic Engineering and Water Resources Management, University
of Technolgy, Aachen, Germany.

Streeter, H. W. and Phelps, E- B. (1925) "A study of the pollution and natural
purification of the Ohio River", US Public Health Service, Washington DC,
Bulletin 146.

Vanoni, V., et al (1975) "Sedimentation Engineering", ASCE Manuals and reports
on engineering practice - No54.

Yang, T. C. (1973) "Incipient Motion and Sediment Transport", ASCE Journal of
Hydraulic Engineering, Vol. 99, No HY10.

The references by Olsen (1991), Chandrashekhar (1994) and Lovoll (1996) can be
obtained by writing to:

Department of Hydraulic and Environmental Engineering
The Norwegian University of Science and Technology
N-7034 Trondheim
Norway

The proceedings with reference by Olsen and Alfredsen (1994) can be obtained by
writing to:

SINTEF Civil and Environmental Engineering
Klaebuvn. 153
N-7034 Trondheim
Norway

The thesis by Sintic (1996) can be obtained by writing to:

RWTH Aachen
Institut fur Wasserbau und Wasserwirtschaft
Mies-van-der-Rohe-Str. 1
52056 Aachen
Germany


ΓòÉΓòÉΓòÉ 8.1. Velocity vector map - Garita ΓòÉΓòÉΓòÉ

The colors show the magnitude of the horizontal velocity