(a)
Start-up commands:
SWASH
USER MANUAL
SWASH version 10.05A
| by | : | The SWASH team |
| mail address | : | Delft University of Technology |
| Faculty of Civil Engineering and Geosciences | ||
| Environmental Fluid Mechanics Section | ||
| P.O. Box 5048 | ||
| 2600 GA Delft | ||
| The Netherlands | ||
| website | : | http://www.tudelft.nl/swash |
Copyright (c) 2010-2024 Delft University of Technology.
Permission is granted to copy, distribute and/or modify this document under the terms of the GNU Free Documentation License, Version 1.2 or any later version published by the Free Software Foundation; with no Invariant Sections, no Front-Cover Texts, and no Back-Cover Texts. A copy of the license is available at http://www.gnu.org/licenses/fdl.html#TOC1.
The information about the SWASH package is distributed over three different documents. This
User Manual describes the specifications for the input of the SWASH model. The
Implementation Manual explains the installation procedure and the usage of SWASH on a single-
or multi-processor machine with distributed memory. The Scientific/Technical documentation
discusses the physical and mathematical details and the discretizations that are used in the
SWASH program. Apart from these documents, programmers who want to further
develop SWASH can also consult the Programming rules as applied for SWAN; see
http://www.swan.tudelft.nl for further details.
To make this manual more accessible we briefly describe the contents of each chapter. In
Chapter 2 general description of the model and some instructions concerning the usage of
SWASH, the treatment of grids, boundary conditions, etc. are given. It is advised to read
this chapter before consulting the rest of the manual. Chapter 3 gives some remarks
concerning the input and output files of SWASH. Chapter 4 describes the complete
set of commands of the program SWASH. This chapter will be the most consulted
part of the manual. In Chapter 5 some guidelines for setting up a command file is
outlined.
This manual also contains some appendices. In Appendix A definitions of some parameters are
given. Next, Appendix B outlines the syntax of the command file (or input file). Finally, a
complete set of all the commands use in SWASH can be found in Appendix C.
If this is your first time to start working with SWASH we suggest you to first read Chapters 2 and 3. Next, Chapter 5 is recommended to practice the use of SWASH while guiding you through the main steps to set up a wave model.
The purpose of this chapter is to provide the user with relevant background information
on SWASH and to give some general advice in choosing the basic input for SWASH
computations.
A general suggestion is: start simple. SWASH helps in this with default options. Moreover, it is a good idea to read Chapter 5 first when setting up a command file for the first time. Furthermore, suggestions are given that should help the user to choose among the many options conditions and in which mode to run SWASH (1D or flume-like, 2D or basin-like, depth-averaged or multi-layered, etc.). In addition, the way you need to specify the parameters and options resembles to that of SWAN. Hence, those users who are familiar with SWAN should be able to use SWASH without much effort. It is recommended to carry out some available test cases first to get acquaint with the program.
SWASH is a general-purpose numerical tool for simulating non-hydrostatic, free-surface, rotational flows and transport phenomena in one, two or three dimensions. The governing equations are the nonlinear shallow water equations including non-hydrostatic pressure and some transport equations, and provide a general basis for simulating
The model is referred to as a wave-flow model and is essentially applicable in the coastal regions
up to the shore. This has prompted the acronym SWASH for the associated code, standing for
Simulating WAves till SHore. The basic philosophy of the SWASH code is to provide
an efficient and robust model that allows a wide range of time and space scales of
surface waves and shallow water flows in complex environments to be applied. As a
result, SWASH allows for the entire modelling process to be carried out in any area
of interest. This includes small-scale coastal applications, like waves approaching a
beach, wave penetration in a harbour, flood waves in a river, oscillatory flow through
canopies, salt intrusion in an estuary, and large-scale ocean, shelf and coastal systems
driven by Coriolis and meteorological forces to simulate tidal waves and storm surge
floods.
SWASH is close in spirit to SWAN (Simulating WAves Nearshore) with respect to the pragmatism employed in the development of the code in the sense that comprises are sometimes necessary for reasons of efficiency and robustness. On the one hand, it provides numerical stability and robustness, and on the other hand it gives accurate results in a reasonable turn-around time.
The open source code of SWASH has been developed based on the work of Stelling and Zijlema [4], Stelling and Duinmeijer [2], Zijlema and Stelling [6, 7], Smit et al. [1], Zijlema et al. [8] and Zijlema [5]. The main elements of the SWASH code are:
Like SWAN, the software package of SWASH includes user-friendly pre- and post-processing and does not need any special libraries (e.g. PETSc, HYPRE). In addition, SWASH is highly flexible, accessible and easily extendible concerning several functionalities of the model. As such, SWASH can be used operationally and the software can be used freely under the GNU GPL license (https://swash.sourceforge.io).
SWASH is a free-surface, terrain-following, multi-dimensional hydrodynamic simulation model to
describe unsteady, rotational flow and transport phenomena in coastal waters as driven by e.g.,
waves, tides, buoyancy and wind forces. It solves the continuity and momentum equations, and
optionally the equations for conservative transport of salinity, temperature and suspended load
for both noncohesive sediment (e.g. sand) and cohesive sediment (mud, clay, etc.). In addition,
the vertical turbulent dispersion of momentum and diffusion of salt, heat and suspended
sediment are calculated by means of the standard k − 𝜀 turbulence model. The transport
equations are coupled with the momentum equations through the baroclinic forcing term,
whereas the equation of state is employed that relates density to salinity, temperature and
suspended sediment.
SWASH accounts for the following physical phenomena:
The model has been validated with a series of analytical, laboratory and field test cases.
Overall, the level of agreement between predictions and observations is quite favourable,
particularly in view of the fact that a wide range of wave conditions and topographies were
modelled.
SWASH is proved to reproduce the main features of surf zone dynamics, such as nonlinear
shoaling, wave breaking, wave runup and wave-driven currents. For instance, considering a
typical surf zone where the dominant processes of triad interaction and depth-induced breaking
can be isolated, it was found that the model yields a realistic representation of the observed
frequency spectra, including the overall spectral shape at frequencies above the spectral peak,
and the inclusion of subharmonics. This is followed by a transformation toward a broadband
spectral shape as the waves approach the shoreline.
Such phenomena appear to be rooted in the ability of the staggered (covolume) momentum-conservative scheme to mimic the dynamics within travelling bores associated with wave breaking across the surf zone. In addition, because of the use of discrete analogs of the physical properties of the governing PDEs (e.g. topology, flux conservation) the effect of discretization error originated from the discretization approximations is thus limited, in that the numerical solution is merely influenced by the mesh resolution and mesh quality. Also, the employed SWASH scheme rules out non-physical artefacts that can occur when using a traditional discretization approach (e.g. finite volume methods).
SWASH is not a Boussinesq-type wave model. In fact, SWASH may either be run in
depth-averaged mode or multi-layered mode in which the three-dimensional computational
domain is divided into a fixed number of vertical terrain-following layers. SWASH improves its
frequency dispersion by increasing this number of layers rather than increasing the order of
derivatives of the dependent variables like Boussinesq-type wave models. Yet, it contains at most
second order spatial derivatives, whereas the applied finite difference approximations are at most
second order accurate in both time and space.
In addition, SWASH does not have any numerical filter nor dedicated dissipation mechanism to eliminate short wave instabilities. Neither does SWASH include other ad-hoc measures like the surface roller model for wave breaking, the slot technique for moving shoreline, and the alteration of the governing equations for modelling wave-current interaction. As such, SWASH is very likely to be competitive with the extended Boussinesq-type wave models in terms of robustness and the computational resource required to provide reliable model outcomes in challenging wave and flow conditions. Therefore, it can be seen as an attractive alternative to the Boussinesq-type wave models.
SWASH is a non-hydrostatic wave-flow model and is originally designed for wave transformation
in coastal waters. However, with the extension of meteorological and baroclinic forcing and solute
transport (since version 2.00), this model is capable of using for large-scale flow and transport
phenomena driven by tidal, wind and buoyancy forces. In this respect, SWASH is very similar to
other traditional hydrodynamic models, such as WAQUA, Delft3D-FLOW, ADCIRC,
ROMS, FVCOM, UNTRIM, SLIM and SUNTANS. They mainly differ in numerics and
geometric flexibility, though SWASH supports unstructured triangular grids (since version
7.01).
The need to accurately predict small-scale coastal flows and transport of contaminants
encountered in environmental issues is becoming more and more recognized. The aforementioned
models, however, are orginally designed to simulate large-scale circulation. The development of
these models is often dictated by model limitations, numerical techniques and computer
capabilities. For instance, the hydrostatic pressure assumption prohibits the models to
appropriately simulate surface waves, internal waves, and small-scale flows around hydraulic
structures.
In principle, SWASH has no limitations and can capture flow phenomena with spatial scales from centimeters to kilometers and temporal scales from seconds to hours. Yet, this model can be employed to resolve the dynamics of wave transformation, buoyancy flow and turbulent exchange of momentum, salinity, heat and suspended sediment in shallow seas, coastal waters, surf zone, estuaries, reefs, rivers and lakes.
Sometimes the user input to SWASH is such that the model produces unreliable or unstable results. This may be the case, for instance, if the bathymetry is not well resolved or the boundary conditions are wrong (not well-posed). In addition, SWASH may invoke some internal scenarios instead of terminating the computations. The reasons for this model policy is that
Examples are:
Some other problems which the SWASH user may encounter are due to more fundamental
shortcomings, e.g., turbulence modelling, and unintentional coding bugs.
Because of the issues described above, the results may look realistic, but they may (locally) not be accurate. Any change in these scenarios or shortcomings, in particular newly discovered coding bugs and their fixes, are published on the SWASH website and implemented in new releases of SWASH.
SWASH expects all quantities that are given by the user to be expressed in S.I. units: m, kg, s
and composites of these with accepted compounds, such as Newton (N) and Pascal (Pa).
Consequently, the water level and water depth are in m, flow velocity in m/s, etc. For wind,
(incident) wave and flow direction both the Cartesian and a nautical convention can be
used (see below). Directions and spherical coordinates are in degrees (0) and not in
radians.
SWASH operates either in a Cartesian coordinate system or in a spherical coordinate system, i.e.
in a flat plane or on a spherical Earth. In the Cartesian system, all geographic locations and
orientations in SWASH, e.g. for the bottom grid or for output points, are defined in one common
Cartesian coordinate system with origin (0,0) by definition. This geographic origin may be
chosen totally arbitrarily by the user. In the spherical system, all geographic locations and
orientations in SWASH, e.g. for the bottom grid or for output points, are defined in geographic
longitude and latitude. Both coordinate systems are designated in this manual as the problem
coordinate system.
In the input and output of SWASH the direction of wind, (incident) wave and current are defined according to either
All other directions, such as orientation of grids, are according to the Cartesian convention!
For regular grids, i.e. uniform and rectangular, Figure 4.1 (in Section 4.5) shows how the locations of the various grids are determined with respect to the problem coordinates. All grid points of curvilinear and unstructured grids are relative to the problem coordinate system.
Both spatial grids and time windows need to be defined.
The spatial grids that need to be defined by the user are (if required):
Wind, bottom friction, grain sizes, heights of porous structures and vegetation density do not require
a grid if they are uniform over the area of interest.
For one-dimensional situations, i.e. ∂∕∂y ≡ 0, SWASH can be run in 1D mode.
If a uniform, rectangular computational grid is chosen in SWASH, then all input and output
grids must be uniform and rectangular too, but they may all be different from each
other.
If an orthogonal curvilinear computational grid is chosen in SWASH, then each input grid
should be either uniform, rectangular or identical to the used curvilinear computational
grid.
If an unstructured computational spatial grid is chosen in SWASH, then each input grid should
be either uniform, rectangular or identical to the used unstructured grid.
Also, SWASH may operate with different time windows with different time steps (each may have a different start and end time and time step):
During the computation SWASH obtains bottom, current, water level, wind, pressure, bottom friction, porosity, grain size, structure height and vegetation density information by tri-linear interpolation from the given input grid(s) and time window(s). The output is in turn obtained in SWASH by bi-linear interpolation in space from the computational grid; there is no interpolation in time, the output time is shifted to the nearest computational time level. Interpolation errors can be reduced by taking the grids and windows as much as equal to one another as possible (preferably identical). It is recommended to choose output times such that they coincide with computational time levels.
The computational grid must be defined by the user. The orientation (direction) can be
chosen arbitrarily.
If the computational grid extends outside the input grid, the reader is referred to Section 2.5.3
to find the assumptions of SWASH on depth, current, water level, wind, bottom friction,
porosity, grain size, structure height and vegetation density in the non-overlapping
area.
The spatial resolution of the computational grid should be sufficient to resolve relevant details of
the wave field. Usually a good choice is to take the resolution of the computational grid
approximately equal to that of the bottom or current grid. See Chapter 5 for further
details.
Alternatively, the user may apply a curvilinear, boundary-fitted grid. This grid must be
orthogonal, but may either be uniform or non-uniform. The domain boundaries may be curved.
The exception is when a wave spectrum is imposed, in which case the wavemaker boundaries
must be non-curved (see also Chapter 5 for details).
If necessary, an unstructured triangular grid may be used for a further extensive local mesh
refinements (e.g. in the surf zone).
SWASH may not use the entire user-provided computational grid if the user defines exception values on the bottom grid (see command INPGRID BOTTOM) or on the curvilinear computational grid (see command CGRID). A computational grid point is either
It must be noted that for parallel runs using MPI the user must indicate an exception value when
reading the bottom levels (by means of command INPGRID BOTTOM EXCEPTION), if appropriate,
in order to obtain good load balancing.
For further suggestions regarding choice of the resolution and orientation of the computational
grid the user is kindly referred to Chapter 5.
The computational time window must be defined by the user. The computational window in
time must start at a time that is early enough that the initial state of SWASH has
propagated through the computational area before reliable output of SWASH is expected.
Before this time the output may not be reliable since usually the initial state is not
known.
The computational time step must be given by the user. Since, SWASH is based on explicit schemes, it is limited by a Courant stability criterion (which couples time and space steps). Moreover, the accuracy of the results of SWASH are obviously affected by the time step. Generally, the time step in SWASH should be small enough to resolve the time variations of computed wave field itself. Usually, it is enough to consider the time variations of the wave boundary conditions.
The bathymetry, current, water level, bottom friction (if spatially variable), wind (if spatially
variable), atmospheric pressure, porosity regions, grain sizes, heights of porous structures (if
spatially variable) vegetation density (if spatially variable) and drafts (and optionally labels) of
floating objects (e.g. moored ships, WECs) need to be provided to SWASH on so-called input
grids. It is best to make an input grid so large that it completely covers the computational
grid.
When the atmospheric pressure is included, it must be combined with space varying wind. They
may be read from a meteorological file. Space varying wind and pressure is of particular
importance for the simulation of storm surges.
In the region outside the input grid SWASH assumes that the bottom level, the water
level, bottom friction, atmospheric pressure, stone diameter and vegetation density
are identical to those at the nearest boundary of the input grid (lateral shift of that
boundary). In the regions not covered by this lateral shift (i.e. in the outside quadrants
of the corners of the input grid), a constant field equal to the value at the nearest
corner point of the input grid is taken. For the current and wind velocity, SWASH
takes 0 m/s for points outside the input grid, while for porosity and structure height,
SWASH takes 1 and 99999 (i.e. emerged), respectively, for points outside the input
grid.
One should choose the spatial resolution for the input grids such that relevant spatial details in
the bathymetry, current, bottom friction, wind and pressure and floating objects are properly
resolved. Special care is required in cases with sharp and shallow ridges (sand bars, shoals,
breakwaters) in the sea bottom and extremely steep bottom slopes. Very inaccurate bathymetry
can result in very inaccurate wave transformation or flooding and drying. In such
cases the ridges are vitally important to obtain good SWASH results. This requires
not only that these ridges should be well represented on the input grid but also after
interpolation on the computational grid. This can be achieved by choosing the grid
lines of the input grid along the ridges (even if this may require some slight ”shifting”
of the ridges) and choosing the computational grid to be identical to the input grid
(otherwise the ridge may be ”lost” in the interpolation from the bottom input grid to the
computational grid). An alternative is to smooth the bottom gradients. But this should be
done in a way that the quality and feature of the bathymetric data is more or less the
same.
In SWASH, wind, pressure and bottom friction may be time varying. In that case they need to
be provided to SWASH in so-called input time windows (they need not be identical with the
computational, output or other input windows). It is best to make an input window larger than
the computational time window. SWASH assumes zero values at times before the earliest begin
time of the input parameters (which may be the begin time of any input parameter such as
wind). SWASH assumes constant values (the last values) at times after the end time of each
input parameter. The input windows should start early enough so that the initial state of
SWASH has propagated through the computational area before reliable output of SWASH is
expected.
Finally, one should use a time step that is small enough that time variations in the wind, pressure and bottom friction are well resolved.
With SWASH some transport phenomena of constituents can be simulated that result from tidal,
wind and wave forcing in stratified flows. The considered constituents are salinity, temperature
and suspended sediment load. The presence of these constituents will influence the density of
water and consequently, they will induce flow through the baroclinic pressure gradient. In this
way, transport of constituents and water flow are coupled. Examples are salt intrusion in an
estuary, sediment transport in turbidity flows and transport of dissolved matter in lakes and
rivers.
Only the background temperature is considered in the model, and the heat exchange flux at the
air-water interface is not taken into account.
With respect to the sediment transport, the following assumptions are made.
The inclusion of transport of constituent in SWASH must be done by means of an input grid for
each constituent. Such an input grid represents the ambient or background concentration of the
corresponding constituent as an initial state, while it provides information along the open
boundaries of the computational domain. The use of this information to impose a boundary
condition for constituent depends on the flow direction. At inflow, the concentration is prescribed
using this information delivered by the input grid. At outflow, the concentration is determined
solely by the concentration in upstream part of the domain due to pure advection. It is
assumed that the area of interest in which transport phenomena occur is far away
from the open boundaries. The ambient concentration at open boundaries is therefore
supposed to be steady state. However, for unsteady salt intrusion in a tidal inlet,
the concentration is prescribed at inflow by means of a so-called Thatcher-Harleman
boundary condition. In this way, a smooth (sinusoidal) transition from the outflow
concentration to the inflow boundary condition can be described; see also command
TRANSPORT.
It is advised to make an input grid so large that it completely covers the computational grid.
Otherwise, SWASH assumes that in the region outside the input grid, the constituent
equals to the value at the nearest boundary of the input grid (lateral shift of that
boundary).
Finally, both the initial state and boundary conditions of any constituent may be vary in the vertical direction. This needs to be provided to SWASH with an input grid for each vertical layer.
SWASH can provide output on uniform, rectilinear grids that are independent from the input
grids and from the computational grid. In the computation with an orthogonal curvilinear
computational grid, curvilinear output grids are available in SWASH. An output grid has to be
specified by the user with an arbitrary resolution, but it is of course wise to choose a resolution
that is fine enough to show relevant spatial details. It must be pointed out that the information
on an output grid is obtained from the computational grid by bi-linear interpolation
(output always at computational time level). This implies that some inaccuracies are
introduced by this interpolation. It also implies that bottom or wind information on an
output plot has been obtained by interpolating twice: once from the input grid to
the computational grid and once from the computational grid to the output grid. If
the input, computational and output grids are identical, then no interpolation errors
occur.
In the regions where the output grid does not cover the computational grid, SWASH assumes
output values equal to the corresponding exception value. For example, the default exception
value for the surface elevation is −99. The exception values of output quantities can be changed
by means of the QUANTITY command.
Output can be requested at regular intervals starting at a given time always at computational times.
The boundaries of the computational grid in SWASH are either land, beach or water. SWASH provides the following specification of boundary conditions:
different wavemakers:
When imposing irregular waves at a boundary segment by means of a spectrum it is assumed that
the variation of the depth along the boundary segment is slowly.
SWASH has the option to make a computation that is nested in SWAN. In such a run, SWASH interpolates the locations, as specified in the SWAN run with POINTS or CURVE, to the user-defined boundary, either side or segment (see command BOUNDCOND), of the concerning SWASH run. The SWAN spectra are written to those locations using the SWAN command SPECOUT. These wave spectra are employed as boundary conditions using the SPECSWAN command. It is assumed that the wave spectra are stationary. Also, both SWASH and SWAN runs must used the same coordinate system, either Cartesian or spherical.
SWASH employs the following time notation: hhmmss.msc with hh, mm, ss and msc denoting hours, minutes, seconds and milliseconds, respectively. Alternatively, SWASH can run for dates
Sometimes SWASH produces an error message concerning an instability due to the fact that the water level is below the bottom level and stops. It is general difficult to find the cause of this problem. However, some suggestions about possible reasons and what to do in such cases are given below.
SWASH is one single computer program. The names of the files provided by the user should
comply with the rules of file identification of the computer system on which SWASH
is run. In addition: SWASH does not permit file names longer than 36 characters.
Moreover,
the maximum length of the lines in the input files for SWASH is 180 positions.
The user should provide SWASH with a number of files (input files) with the following information:
To assist in making the command file, an edit file is available to the user (see Appendix C). In
its original form this file consists only of comments; all lines begin with exclamation mark.
In the file, all commands as given in this User Manual (Chapter 4) are reproduced
as mnemonics for making the final command file. Hence, the user does not need to
consult the User Manual every time to check the correct spelling of keywords, order of
data, etc. The user is advised to first copy the edit file (the copy file should have a
different name) and then start typing commands between the comment lines of the edit
file.
SWASH is fairly flexible with respect to output processing. Output is available for many different quantities. However, the general rule is that output is produced by SWASH only at the user’s request. The instructions of the user to control output are separated into three categories:
SWASH always creates a print file. Usually the name of this file is identical to the name of the
command file of the computations with the extension (.SWS) replaced with (.PRT). Otherwise, it
depends on the batch file that is used by the user. Consult the Implementation Manual for more
information.
The print file contains an echo of the command file, an overview of the actual physical and
numerical parameters to be used in the simulation run, and possibly warning and error messages.
These messages are usually self-explanatory. The print file also contains computational results if
the user so requests (with command BLOCK or TABLE).
IN ANY CASE, ALWAYS CHECK THE PRINT FILE!
The following commands are available to users of SWASH (to look for the commands quickly, see
table of contents and index).
Start-up commands
(a)
Start-up commands:
Commands for model description
(b)
Commands for computational grid:
(c)
Commands for input fields:
(d)
Commands for initial and boundary conditions:
(e)
Commands for physics:
(f)
Commands for numerics:
Output commands
(g)
Commands for output locations:
(h)
Commands to write or plot output quantities:
(i)
Commands to write or plot intermediate results:
Lock-up commands
(j)
Commands to lock-up the input file:
SWASH executes the above command blocks (a,...,j) in the above sequence except (f), (i) and (j).
The commands of the blocks (f) and (i) may appear anywhere before block (j), except that TEST
POINTS must come after READINP BOTTOM. The commands of block (j) may appear anywhere in
the command file (all commands after COMPUTE are ignored by SWASH, except STOP). A
sequence of commands of block (g) is permitted (all commands will be executed without
overriding). Also a sequence of commands of block (h) is permitted (all commands will be
executed without overriding).
Within the blocks the following sequence is to be used:
It must be noted that a repetition of a command may override an earlier occurrence of that
command.
Many commands provide the user with the opportunity to choose an option (e.g. discretization
scheme) or assign values to coefficients (e.g. bottom friction coefficient). If the user does not use
such option SWASH will use a default value.
Some commands cannot be used in 1D-mode and in case of unstructured grids (see individual command descriptions below).
The command syntax is given in Appendix B.
Limitations:
PROJect ’name’ ’nr’ ’title1’ ’title2’ ’title3’
With this required command the user defines a number of strings to identify the SWASH run (project name e.g., an engineering project) in the print and plot file.
SET [level] [nor] [depmin] [maxmes] [maxerr] [seed] & [grav] [rhowat] [temp] [salinity] [dynvis] [rhoair] [rhosed] & [cdcap] [prmean] [backvisc] [kappa] & | NAUTical | CORIolis < > [outlev] | -> CARTesian |
With this optional command the user assigns values to various general parameters.
| | |-> TWODimensional | MODE < NONSTationary > < > | | | ONEDimensional |
With this optional command the user indicates that the run will be either one-dimensional
(1D-mode, flume) or two-dimensional (2D-mode, basin).
Note that the keyword NONSTATIONARY is obliged.
The default option is NONSTATIONARY TWODIMENSIONAL.
| -> CARTesian COORDINATES < | -> CCM | SPHErical < | QC
Command to choose between Cartesian and spherical coordinates (see Section 2.4).
Note that spherical coordinates can also be used for relatively small areas, say 10 or 20 km
horizontal dimension. This may be useful if one obtains the boundary conditions by nesting in an
oceanic model which is naturally formulated in spherical coordinates.
Note that in case of spherical coordinates regular grids must always be oriented E-W, N-S, i.e. [alpc]=0, [alpinp]=0, [alpfr]=0 (see commands CGRID, INPUT GRID and FRAME, respectively). In addition, spherical coordinates are not supported in case of unstructured grids.
| -> REGular [xpc] [ypc] [alpc] [xlenc] [ylenc] [mxc] [myc] | | | CGRID < CURVilinear [mxc] [myc] (EXCeption [xexc] [yexc]) > & | | | UNSTRUCtured | | -> X REPeating < | Y
With this required command the user defines the geographic location, size, resolution and orientation of the computational grid in the problem coordinate system (see Section 2.5.2) in case of a uniform, rectilinear computational grid, an orthogonal curvilinear grid or an unstructured triangular mesh. The origin of the regular grid and the direction of the positive x−axis of this grid can be chosen arbitrary by the user.
![REGULAR this option indicates that the computational grid is to be taken as uniform and
rectangular.
CURVILINEAR this option indicates that the computational grid is to be taken as curvilinear.
The user must provide the coordinates of the grid points with command
READGRID COOR.
UNSTRUCTURE this option indicates that the computational grid is to be taken as unstructured.
The user must provide the coordinates of the vertices and the numbering of
triangles with the associated connectivity table with vertices with command
READGRID UNSTRUC.
[xpc ] geographic location of the origin of the computational grid in the problem
coordinate system (x − coordinate, in m). See command COORD.
Default: [xpc ] = 0.0 (Cartesian coordinates).
In case of spherical coordinates there is no default, the user must give a value.
[ypc ] geographic location of the origin of the computational grid in the problem
coordinate system (y − coordinate, in m). See command COORD.
Default: [ypc ] = 0.0 (Cartesian coordinates).
In case of spherical coordinates there is no default, the user must give a value.
[alpc ] direction of the positive x− axis of the computational grid (in degrees, Cartesian
convention). In 1D -mode, [alpc ] should be equal to the direction [alpinp ]
(see command INPGRID ).
Default: [alpc ] = 0.0
[xlenc ] length of the computational grid in x − direction (in m ). In case of spherical
coordinates [xlenc ] is in degrees.
[ylenc ] length of the computational grid in y− direction (in m ). In 1D -mode, [ylenc ]
should be 0. In case of spherical coordinates [ylenc ] is in degrees.
[mxc ] number of meshes in computational grid in x− direction for a uniform, rectilinear
grid or ξ− direction for a curvilinear grid (this number is one-less than the
number of grid points in this domain! ).
[myc ] number of meshes in computational grid in y− direction for a uniform, rectilinear
grid or η − direction for a curvilinear grid (this number is one-less than the
number of grid points in this domain! ). In 1D -mode, [myc ] should be 0.
EXCEPTION only available in the case of a curvilinear-grid. If certain grid points are to be
ignored during the computation (e.g. land points that remain dry i.e. no
flooding; saving computer time and memory ), then this can be indicated by
identifying these grid points in the file containing the grid point coordinates
(see command READGRID ). For an alternative, see command INPGRID BOTTOM.
[xexc ] the value which the user uses to indicate that a grid point is to be ignored
in the computations (this value is provided by the user at the location of the
x− coordinate considered in the file of the x− coordinates, see command
READGRID COOR). Required if the option EXCEPTION is used.
Default: [xexc ] = 0.0
[yexc ] the value which the user uses to indicate that a grid point is to be ignored
in the computations (this value is provided by the user at the location of the
y− coordinate considered in the file of the y − coordinates, see command
READGRID COOR). Required if the option EXCEPTION is used.
Default: [yexc ] = [xexc ]
REPEATING this option indicates that the grid is repeated in one specific direction.
It means that information leaving at one end of the domain enters at
the opposite end. So, the current or wave field is periodic in one direction
with the length of the domain in that direction.
NOT FOR 1D--MODE--- AND UNSTRUCTURED--------GRIDS.--
X the computational grid is repeated in x − or ξ− direction.
This is default.
Y the computational grid is repeated in y− or η− direction.](swashuse24x.svg)
For illustration of a regular grid with its dimensions, see Figure 4.1.
READgrid COORdinates [fac] ’fname’ [idla] [nhedf] [nhedvec] & | -> FREe | | | | | ’form’ | | < FORmat < > > | | [idfm] | | | | | UNFormatted |
CANNOT BE USED IN 1D-MODE.
This command READGRID COOR must follow a command CGRID CURV. With this command (required if the computational grid is orthogonal curvilinear; not allowed in case of a regular grid) the user controls the reading of the coordinates of the computational grid points. These coordinates must be read from a file as a vector (x−coordinate, y−coordinate of each single grid point). See command READINP for the description of the options in this command READGRID. SWASH will check whether all angles in the grid are > 0 and < 180 degrees. If not, it will print an error message giving the coordinates of the grid points involved. It is recommended to use grids with angles between 45 and 135 degrees.
| -> TRIAngle | READgrid UNSTRUCtured < > ’fname’ | EASYmesh |
CANNOT BE USED IN 1D-MODE.
This command READGRID UNSTRUC must follow a command CGRID UNSTRUC. With this command (required if the computational grid is unstructured which must be Delaunay; not allowed in case of a regular or curvilinear grid) the user controls the reading of the (x,y) co-ordinates of the vertices including boundary markers and a connectivity table for triangles (or elements). This table contains three corner vertices around each triangle in counterclockwise order. This information should be provided by a number of files generated by one of the following grid generators currently supported by SWASH:
These generators produce Delaunay-type grids. After setting up the vertices and the connectivity tables for cells and faces (automatically done in SWASH), SWASH will print some information concerning the used mesh, among others, number of vertices, cells and faces and minimum and maximum gridsizes.
| M VERTical [kmax] < [thickness] < > | -> PERC
With this optional command the user indicates that the run will be in multi-layered mode and controls the distribution of vertical layers.
![[kmax ] number of vertical layers.
[thickness ] layer thickness (in meters or as percentage of water depth ).
M thickness is given in meters. This layer has a fixed thickness.
PERC thickness is given as percentage. This layer has a variable thickness.
This is default.](swashuse32x.svg)
Notes:
![[level ] still water level (in m ).
Default: [level ]=0.
[nor ] direction of North with respect to the x− axis (measured counterclockwise );
default [nor]= 90o, i.e. x − axis of the problem coordinate system
points East.
When spherical coordinates are used (see command COORD ) the value
of [nor] may not be modi fied.
[depmin ] threshold water depth (in m ). Any grid point with water depth smaller than
[depmin ] is taken out of the computation.
Default: [depmin ] = 0.00005
[maxmes ] maximum number of error messages (not necessarily the number of errors!)
during the computation at which the computation is terminated. During the
computational process messages are written to the PRINT file.
Default: [maxmes ] = 200
[maxerr ] during pre-processing SWASH checks input data. Depending on the severity
of the errors encountered during this pre-processing, SWASH does not start
computations. The user can influence the error level above which SWASH will
not start computations (at the level indicated the computations will continue ).
The error level [maxerr ] is coded as follows:
1 : warnings,
2 : errors (possibly automatically repaired or repairable by SWASH ),
3 : severe errors.
Default: [maxerr ] = 1
[seed ] is the seed of the random number generator used to select phase angles
for the different Fourier components. By selecting different seeds different
time series can be obtained from the same wave spectrum (see command
BOUNDCOND ).
Default: [seed ] = 12345678.
2
[grav ] is the gravitational acceleration (in m/s ).
Default: [grav ] = 9.81
[rhowat ] is the density of water (in kg/m3 ).
Default: [rhowat ] = 1000.
Note: this is usually the reference density. The actual density depends on
the temperature and salinity of water. o
[temp ] is the (ambient ) temperature of water (in C ).
Default: [temp ] = 14.
[salinity ] is the (ambient ) salinity of water (in ppt).
Default: [salinity ] = 31.
[dynvis ] is the dynamical viscosity of water (in kg/ms ).
Default: [dynvis ] = 0.001
[rhoair ] is the density of air (in kg/m3 ).
Default: [rhoair ] = 1.205
[rhosed ] is the density of sediment (in kg/m3 ).
Default: [rhosed ] = 2650.
[cdcap ] is the maximum value for the wind drag coefficient. A value of [cdcap ] = 99999
means no cutting off the drag coefficient. A suggestion for this parameter is
[cdcap ] = 2.5× 10−3.
Default: [cdcap ] = 99999.
2
[prmean ] is the mean atmospheric pressure (in N/m ). This will be used to correct the
water level along the water level boundaries so that it is consistent with the
local atmospheric pressure. A value of [prmean ] = − 1 means no correction.
Default: [prmean ] = − 1.
2
[backvisc ] is the background viscosity (in m /s). It may be convenient to specify this
ambient viscosity to account for all forms of unresolved vertical mixing.
The value must be small compared to the vertical viscosity calculated by the
standard k − 𝜀 model. Experiences suggest a value of 10− 4 to 10− 3 m2/s.
Default: [backvisc ] = 0.
[kappa ] is the Von Karman constant.
Default: [kappa ] = 0.4
CORIOLIS indicates that the Coriolis force will be included.
NAUTICAL indicates that the Nautical convention for wind and current direction (SWASH
input and output ) and for incident wave boundary condition will be used
instead of the default Cartesian convention. For definition, see Section 2.4
or Appendix A.
CARTESIAN indicates that the Cartesian convention for wind and current direction (SWASH
input and output ) and for incident wave boundary condition will be used.
For definition, see Section 2.4 or Appendix A.
[outlev ] defines the amount of output for iterative solvers.
It is coded as follows:
0 : no output,
1 : only fatal errors will be printed,
2 : gives output concerning the iteration process,
3 : additional information about the iteration is printed.
Default: [outlev ] = 0](swashuse16x.svg)
| BOTtom |
| |
| WLEVel |
| |
| | CURrent |
| < |
| | VX |
| | VY |
| |
| FRiction |
| |
| | WInd |
| < |
| | WX |
INPgrid (< | WY >) &
| |
| PRessure |
| |
| POROsity |
| |
| PSIZe |
| |
| HSTRUCture |
| |
| NPLAnts |
| |
| DRAFt |
| |
| LABel |
| -> REGular [xpinp] [ypinp] [alpinp] [mxinp] [myinp] [dxinp] [dyinp] |
| |
< CURVilinear STAGgered > &
| |
| UNSTRUCtured |
(EXCeption [excval]) &
| -> Sec |
(NONSTATionary [tbeginp] [deltinp] < MIn > [tendinp])
| HR |
| DAy |
OPTION CURVILINEAR AND UNSTRUCTURED NOT FOR 1D-MODE.
With this required command the user defines the geographic location, size and orientation of an
input grid and also the time characteristics of the variable if it is not stationary. If this is the case
(the variable is not stationary), the variable should be given in a sequence of fields, one for each
time step [deltinp]. The actual reading of values of bottom, wind, pressure, etc. from file is
controlled by the command READINP.
This command INPGRID must precede the following command READINP.
There can be different grids for bottom level (BOTTOM), current (CURRENT), bottom friction
coefficient (FRICTION), wind velocity (WIND), atmospheric pressure (PRESSURE), porosity layers
(POROSITY), stone diameters (PSIZE), heights (HSTRUCTURE) of porous structures and vegetation
density (NPLANTS) and drafts/labels of floating objects like a vessel or WECs (DRAFT and
LABEL).
If the current velocity components are available on different grids, then option VX, VY can define
these different grids for the x− and y−component of the current, respectively (but the grids
must have identical orientation). Different grids for VX and VY may be useful if the data are
generated by a circulation model using a staggered grid. The same holds for the wind velocity
components, i.e. WX and WY.
In the case of a regular grid (option REGULAR in the INPGRID command) the current and wind
velocity vectors are defined with the x− and y−component of the current or wind vector with
respect to the x−axis of the input grid. In case of an orthogonal curvilinear grid (option
CURVILINEAR in the INPGRID command) the current and wind velocity vectors are defined with
the x− and y−component of the current or wind vector with respect to the x−axis of the
problem coordinate system (see Figure 4.1).
In case of an unstructured grid (option UNSTRUC in the INPGRID command) the current and wind
velocity vectors are defined with the x− and y−component of the current or wind vector with
respect to the x−axis of the problem coordinate system (see Figure 4.1).
Porosity layers can be placed inside the computational domain to simulate reflection and
transmission effects of porous structures such as rubble mound breakwaters and jetties. Porosity
is defined as the volumetric porosity of the structures and its value is in between 0 and 1. A
porosity value of 0.45 is typically used for breakwaters. A small value (< 0.1) should be
interpreted as impermeable, like walls and dams. Also structure heights (relative to
the bottom) can be specified so that both submerged and emerged breakwaters is
allowed.
If the user specifies an input grid for the atmospheric pressure, then an input grid for wind must
be included as well. Both space varying wind and pressure may be read from a meteorological
file.
For wind velocity, friction coefficient, grain size, height of porous structures and vegetation
density it is also possible to use a constant value over the computational field (see commands
WIND, FRICTION, POROSITY and VEGETATION, respectively). No grid definition for wind, friction,
grain size, structure height or vegetation density is then required.
Note that in case of options BOTTOM, POROSITY, PSIZE, HSTRUCTURE, NPLANTS and LABEL only
stationary input field is allowed.
If the computational grid is unstructured, the input grids can be either regular or identical to the
used computational grid.
If land points remain dry during the computation (no flooding!), then these points can be
ignored. In this way, simulation time and internal memory can be saved. This can be done by
indicating bottom level in these points as exception value. See command INPGRID BOTTOM
EXCEPTION. For parallel runs using MPI, an exception value for bottom levels should be
prescribed in order to have a good load-balancing!
Exception value for bottom levels can also be used to take into account dams, screens, quays or
jetties in the domain. In addition, they may represent small obstacles with subgrid dimensions
that possibly influence the local flow pattern. In this way, the user can defined a line of thin
dams that separate the flow on both sides.
See Section 2.5.3 for more information on input grids.
| BOTtom | | | | WLEVel | | | | CURrent | | | | FRiction | | | | WInd | | | | PRessure | | ’fname1’ | READinp < > [fac] < > [idla] & | POROsity | | SERIes ’fname2’ | | | | PSIZe | | | | HSTRUCture | | | | NPLAnts | | | | DRAFt | | | | LABel | | -> FREe | | | | | ’form’ | | [nhedf] ([nhedt]) ([nhedvec]) < FORmat < > > | | [idfm] | | | | | UNFormatted |
With this required command the user controls the reading of values of the indicated variables
from file. This command READINP must follow a command INPGRID.
If the variables are in one file, then the READINP commands should be given in the same sequence as the sequence in which the variables appear in the file.
![BOTTOM with this option the user indicates that bottom levels (in m) are to be read from
file (bottom level positive downward relative to an arbitrary horizontal datum
level). The sign of the input can be changed with option [fac ] = − 1. (see below ).
WLEV with this option the user indicates that water levels (in m ) are to be read from
file (water level positive upward relative to the same datum level as used in
option BOTTOM ). Sign of input can be changed with option [fac] = − 1. If the
water level is constant in space and time, the user can use the command SET
to add this (still) water level to the still water depth.
CURRENT rectilinear (curvilinear) input grid: with this option the user indicates that
----------------------------------
the x− and y− component (ξ− and η− component ) (in m/s ) are to be read from
one and the same file (with one READINP command ). With this option SWASH
reads first all x− components (ξ− components ), and then all y− components
(η− components ) (see [idla] ). The first component (x− or ξ− component ) is
always eastward oriented and the second one (y− or η− component ) is always
northward oriented. There is one exception: in case of rotated rectilinear grid,
the x− and y− components are taken along the direction of the grid lines.
unstructured-input-grid: with this option the user indicates that the x− and
y− component (in m/s ) are to be read from one and the same file (with one
READINP command ). With this option SWASH reads first all x − components,
and then all y− components. The order of these values to be read is identical
to that of the unstructured computational grid.
FRICTION with this option the user indicates that friction coefficient is to be read from
file for Manning or Chezy formula’s or Nikuradse roughness height. If the
coefficients are constant in space and time: see command FRICTION.
WIND rectilinear (curvilinear) input grid: with this option the user indicates that
the x− and y− component (ξ− and η− component ) (in m/s ) are to be read from
one and the same file (with one READINP command ). With this option SWASH
reads first all x− components (ξ− components ), and then all y− components
(η− components ) (see [idla] ). The first component (x− or ξ− component ) is
always eastward oriented and the second one (y− or η− component ) is always
northward oriented. There is one exception: in case of rotated rectilinear grid,
the x− and y− components are taken along the direction of the grid lines.
If the wind is constant, see command WIND.
2
PRESSURE with this option the user indicates that atmospheric pressures (in N/m ) are
to be read from file. Unit can be changed with option [fac] (see below).
POROSITY with this option the user indicates that volumetric porosity is to be read from
file. Porosity values less than 1 indicates the location of porous structures. A
value of 1 represents water points. Regions with small porosity values (< 0.1)
will be treated as impermeable regions, i.e. land points.
PSIZE with this option the user indicates that grain sizes (in m) of porous structures
are to be read from file. If the grain size is constant for all porous structures
then see command POROSITY for specification.
HSTRUCTURE with this option the user indicates that heights (in m ) of porous structures
(relative to the bed level) are to be read from file. If the height is constant
for all porous structures then see command POROSITY for specification.
NPLANTS with this option the user indicates that horizontally varying vegetation
density (per m2) is to be read from file. If the density is constant then
see command VEGETATION for specifcation.
DRAFT with this option the user indicates that the draft of floating object (in m) is
to be read from file (draft positive downward relative to an arbitrary horizontal
datum level). The sign of the input can be changed with option [fac ] = − 1.
(see below ).
LABEL with this option the user indicates that the labels of rigid bodies is to be
read from file. It assigns integer values to each of the bodies, starting from 1.
See command BODY DIMENSION for further specification of body dimensions.
[fac ] SWASH multiplies all values that are read from file with [fac ]. For instance
if the bottom levels are given in unit decimeter, one should make [fac]=0.1 to
obtain levels in m. To change sign of bottom level use a negative value of [fac ].
Note that [fac ] = 0 is not allowed!
Default: [fac ]=1.
’fname1 ’ name of the file with the values of the variable.
SERIES with this option (only for MODE NONSTATIONARY ) the user indicates that the
names--of the files containing the nonstationary variable(s) are located in a
separate file with name ’fname2 ’ (see below ).
’fname2 ’ name of file that contains the names--of the files where the variables
are given. These names are to be given in proper time sequence. SWASH reads
the next file when the previous file end has been encountered. In these files the
input should be given in the same format as in the above file ’fname1 ’ (that
implies that a file should start with the start of an input time step).
[idla ] prescribes the order in which the values of bottom levels and other fields
should be given in the file.
=1: SWASH reads the map from left to right starting in the upper -left-hand
corner of the map (it is assumed that the x− axis of the grid is pointing
to the right and the y− axis upwards ). A new line-in the map should
start on a new line-in the file. The lay-out is as follows:
1,myc+1 2,myc+1 ... mxc+1, myc+1
1,myc 2,myc ... mxc+1, myc
... ... ... ...
1,1 2,1 ... mxc+1, 1
=2: as [idla]=1 but a new line in the map need not start on a new line in
the file.
=3: SWASH reads the map from left to right starting in the lower-left-hand
corner of the map. A new line-in the map should start on a new line-in
the file. The lay -out is as follows:
1,1 2,1 ... mxc+1, 1
1,2 2,2 ... mxc+1, 2
... ... ... ...
1,myc+1 2,myc+1 ... mxc+1, myc+1
=4: as [idla]=3 but a new line in the map need not start on a new line
in the file.
=5: SWASH reads the map from top to bottom starting in the lower -left-hand](swashuse38x.svg)
If the file does not contain a sufficient number of data (i.e. less than the number of grid points of the input grid), SWASH will write an error message to the PRINT file, and if [itest]>0 (see command TEST) it will reproduce the data in the PRINT file, using the lay-out according to [idla]=1. This echo of the data to print file is also made if the READINP command is embedded between two TEST commands in the command file as follows:
TEST 120 READINP .... TEST 0
| SALinity | | | INPtrans < TEMPerature > & | | | SEDiment | | -> REGular [xpinp] [ypinp] [alpinp] [mxinp] [myinp] [dxinp] [dyinp] | | | < CURVilinear > & | | | UNSTRUCtured | (EXCeption [excval]) & (NONUNIForm [kmax])
OPTION CURVILINEAR NOT FOR 1D-MODE.
With this command the user defines the geographic location, size and orientation of a stationary
input grid for the transport of constituent. This input grid thus supplies initial and stationary
boundary conditions for the considered constituent. The actual reading of constituent values
from file is controlled by the command READTRANS.
This command INPTRANS must precede the following command READTRANS.
There can be different grids for salinity (SALINITY), temperature or heat (TEMPERATURE) and
suspended sediment load (SEDIMENT).
See command INPGRID for the description of the options in this command INPTRANS.
See Section 2.5.4 for more information on (input) grids for transport of constituents.
| SALinity | | | | ’fname1’ | READtrans < TEMPerature > [fac] < > [idla] & | | | LAYers ’fname2’ | | SEDiment | | -> FREe | | | | | ’form’ | | [nhedf] < FORmat < > > | | [idfm] | | | | | UNFormatted |
With this command the user controls the reading of initial and boundary values of
transport constituents from file. This command READTRANS must follow a command
INPTRANS.
The constituents that can be read are salinity (SALINITY) (in ppt, psu or kg/m3),
temperature (TEMPERATURE) (in oC) and suspended sediment load (SEDIMENT) (in
kg/m3).
See command READINP for the description of the options in this command READTRANS.
| | ACURrent | | < | INPamb < | AVX > & | | AVY | | | | MWL | | -> REGular [xpinp] [ypinp] [alpinp] [mxinp] [myinp] [dxinp] [dyinp] | < > & | CURVilinear STAGgered | (EXCeption [excval]) & (NONUNIForm [kmax])
OPTION CURVILINEAR NOT FOR 1D-MODE.
With this command the user defines the geographic location, size and orientation of a
stationary input grid of the ambient current, such as riverine, tidal and wind-driven
flows, and the associated mean water level. With this input grid the effect of ambient
currents on the wave dynamics is accounted for in the simulation. The ambient current
(ACURRENT) and the corresponding mean water level (MWL) can be spatially varying but are
assumed to be constant in time with respect to the temporal wave motion. The actual
reading of values of ambient current and/or mean water level from file is controlled by
the command READAMB. This command INPAMB must precede the following command
READAMB.
There can be different grids for current (ACURRENT) and mean water level (MWL). Additionally, if
the ambient velocity components are available on different grids, then options AVX and AVY can
define these different grids for the x− and y−component of the ambient current, respectively
(but the grids must have identical orientation).
In the case of a regular grid (option REGULAR) the ambient current is defined with the x− and
y−component of the current vector with respect to the x−axis of the input grid. Hence, these
velocity components are (input) grid oriented.
In case of an orthogonal curvilinear grid (option CURVILINEAR) the current is defined with the
x− and y−component of the current vector with respect to the x−axis of the problem
coordinate system (see Figure 4.1).
See also command INPGRID for the description of the options not described here.
It is also possible to use a constant value over the computational field; see command AMBIENT.
No grid definition for ambient current or mean water level is then required.
This command is not supported in case of unstructured grids.
| ACURrent | | ’fname1’ | READamb < > [fac] < > [idla] & | MWL | | LAYers ’fname2’ | | -> FREe | | | | | ’form’ | | [nhedf] < FORmat < > > | | [idfm] | | | | | UNFormatted |
With this command the user controls the reading of ambient current and the associated mean
water level from file. This command READAMB must follow a command INPAMB.
See also command READINP for the description of the options not described here.
![ACURRENT with this option the user indicates that the x− and y− component (ξ− and
η− component ) (in m/s ) are to be read from one and the same file (with one
READAMB command ). With this option SWASH reads first all x − components
(ξ− components ), and then all y− components (η− components ) (see [idla ]).
The first component (x− or ξ− component ) is always eastward oriented and
the second one (y− or η− component ) is always northward oriented. There is
one exception: in case of rotated rectilinear grid, the x − and y− components
are taken along the direction of the grid lines.
MWL with this option the user indicates that water levels (in m ) are to be read from
file (water level positive upward relative to the same datum level as used in
option READ BOTTOM ). Sign of input can be changed with option [fac] = − 1.
LAYERS with this option (only for multi-layered mode ) the user indicates that the
names--of the files containing the non-uniform ambient current are
resided in a separate file with name ’fname2 ’ (see below ).
’fname2 ’ name of file that contains the names--of the files where the current
are given. These names are to be given in proper sequence, i.e. from top
(first layer) to bottom (last layer). SWASH reads the next file when the
previous file end has been encountered. In these files the input should be
given in the same format as in the above file ’fname1 ’.](swashuse50x.svg)
| -> CONstant [wlev] [vx] [vy] [tke] [epsilon] | INITial < ZERO | | STEAdy
This command can be used to specify the initial values for flow variables.
| PM | | | | -> SIG | | -> PEAK | BOUnd SHAPespec < -> JONswap [gamma] > < > < > & | | | RMS | | MEAN | | TMA | | -> POWer | DSPR < > | DEGRees |
This command BOUND SHAPESPEC defines the shape of the spectra (both in frequency and direction) at the open boundary of the computational grid or in the computational domain using source function for internal wave generation in case of parametric spectral input (see either command BOUNDCOND or command SOURCE).
![PM Pierson-Moskowitz spectrum will be used.
JONSWAP JONSWAP spectrum will be used. This is default.
[gamma ] peak enhancement parameter of the JONSWAP spectrum.
Default: [gamma ]=3.3
TMA A modi fied JONSWAP spectrum for finite depth will be used.
SIG The significant wave height (for definition, see Appendix A ) is used as
the characteristic wave height.
This is default.
RMS The RMS wave height (for definition, see Appendix A ) is used as
the characteristic wave height.
PEAK The peak period is used as the characteristic wave period.
This is default.
MEAN Tm01 (for definition, see Appendix A ) is used as the characteristic wave period.
DSPR option for expressing the width of the directional distribution; the distribution
m
function itself is cos (𝜃).
POWER the directional width is expressed with the power m itself.
This option is default.
DEGREES the directional width is expressed in terms of the directional standard deviation
of the cosm (𝜃) distribution (for definition, see Appendix A ).](swashuse56x.svg)
If this command is not used, the JONSWAP option will be used with [gamma]=3.3 and POWER for
the directional width.
![BOTTOM defines the input grid of the bottom level. (For the definition of the bottom
level, see command READINP ).
WLEV defines the input grid of the water level. (For the definition of the water
level, see command READINP ).
CURRENT defines the input grid of the current field (same grid for x − and y − components ).
VX defines the input grid of the x− component of the current field (different grid
than y− component but same orientation).
VY defines the input grid of the y− component of the current field (different grid
than x − component but same orientation).
FRICTION defines the input grid of the bottom friction coefficient (defined in command
FRICTION, not to be confused with this option FRICTION! ).
WIND defines the input grid of the wind velocity field (same grid for x − and
y− component ).
If neither of the commands WIND and READINP WIND is used it is assumed
that there is no wind.
WX defines the input grid of the x− component of the wind velocity field
(different grid than y− component but same orientation).
WY defines the input grid of the y− component of the wind velocity field
(different grid than x− component but same orientation).
PRESSURE defines the input grid of the atmospheric pressure. (For the definition of
the atmospheric pressure, see command READINP ).
POROSITY defines the input grid of the porosity distribution.
If neither of the commands POROSITY and READINP POROSITY is used it is
assumed that there is no porous structure.
PSIZE defines the input grid of the grain sizes of porous structures.
HSTRUCTURE defines the input grid of the heights of porous structures.
NPLANTS defines input grid of the horizontally varying vegetation density (defined
in command VEGETATION ).
DRAFT defines the input grid of the draft of floating objects. (For the definition
of the draft, see command READINP ).
LABEL defines the input grid of the labelling of rigid bodies. (For the definition
of the labels, see command READINP ).
REGULAR means that the input grid is uniform and rectangular.
[xpinp ] geographic location (x− coordinate) of the origin of the input grid in
problem--coordinates (in m ) if Cartesian coordinates are used or in degrees if
spherical coordinates are use (see command COORD).
Default: [xpinp ] = 0. In case of spherical coordinates there is no default, the
user must give a value.
[ypinp ] geographic location (y− coordinate) of the origin of the input grid in
problem--coordinates (in m ) if Cartesian coordinates are used or in degrees if
spherical coordinates are use (see command COORD).
Default: [ypinp ] = 0. In case of spherical coordinates there is no default, the
user must give a value.
[alpinp ] direction of the positive x− axis of the input grid (in degrees, Cartesian convention).
See command COORD.
Default: [alpinp ] = 0.
[mxinp ] number of meshes in x− direction of the input grid (this number is one-less
than the number of grid points in this direction!).
[myinp ] number of meshes in y− direction of the input grid (this number is one-less-
than the number of grid points in this direction!).
In 1D--mode,- [myinp ] should be 0.
[dxinp ] mesh size in x− direction of the input grid,
in m in case of Cartesian coordinates or
in degrees if spherical coordinates are used, see command COORD.
[dyinp ] mesh size in y− direction of the input grid,
in m in case of Cartesian coordinates or
in degrees if spherical coordinates are used, see command COORD.
In 1D--mode,- [dyinp ] may have any value.
Default: [dyinp ] = [dxinp ].
CURVILINEAR means that the input grid is curvilinear; this option is available only if the
computational grid is curvilinear as well. The input grid is identical
to the computational grid.
NOT FOR 1D--MODE.--
STAGGERED means that the input grid of a grid-oriented (not Cartesian!) velocity
component u or v is staggered in y− or x − direction, respectively.
The velocity components are given in their points of definition according
to the Arakawa C-grid staggering.
NOT FOR 1D--MODE.--
UNSTRUCTURE means that the input grid is unstructured; this option is available only if the
computational grid is unstructured as well. The input grid must be identical
to the computational grid.
NOT FOR 1D -MODE .
-----------
EXCEPTION certain points inside the given grid that are to be ignored during the
computation can be identified by means of an exception value as given in
the corresponding input file as controlled by the command READINP.
NOT FOR 1D--MODE.--
[excval ] exception value; required if the option EXCEPTION is used.
Note: if [fac ] ⁄= 1 (see command READINP ), [excval ] must be given as
[fac ] times the exception value.
NONSTATION the variable is nonstationary (given in a time sequence of fields).
NOT FOR 1D--MODE.--
[tbeginp ] begin time of the first field of the variable, the format is:
1 : ISO -notation 19870530.153000
2 : (as in HP compiler ) ’30− May − 87 15:30:00’
3 : (as in Lahey compiler) 05/30/87.15:30:00
4 : 15:30:00
5 : 87/05/30 15:30:00’
6 : as in WAM 8705301530
7 : 153000.000
This format is installation dependent. See Implementation Manual or ask the
person who installed SWASH on your computer. Default is option 7.
[deltinp ] time interval between fields, the unit is indicated in the next option:
SEC unit seconds
MIN unit minutes
HR unit hours](swashuse35x.svg)
![NONUNIFORM the constituent is non-uniform in vertical.
[kmax ] the number of layers representing the number of input fields as given in
a sequence (see command READTRANS ). This number must be equal to the
number of vertical layers in multi-layered mode (see command VERTICAL )
or 1 (i.e. uniform in vertical).
Default: [kmax ] = 1](swashuse41x.svg)
![ACURRENT defines the input grid of the ambient current (same grid for x− and y− components ).
AVX defines the input grid of the x− component of the ambient current (different grid
than y− component but same orientation).
AVY defines the input grid of the y− component of the ambient current (different grid
than x − component but same orientation).
MWL defines the input grid of the mean water level.
NONUNIFORM the ambient current is non-uniform in vertical.
[kmax ] the number of layers representing the number of input fields as given in
a sequence (see command READAMB ). This number must be equal to the
number of vertical layers in multi-layered mode (see command VERTICAL )
or the number of pressure layers in case of the subgrid approach (see
command NONHYD SUBGRID [pmax ]) or 1, that is, uniform in vertical.
Default: [kmax ] = 1](swashuse47x.svg)
![CONSTANT the initial flow and turbulence quantities are set to a constant.
[wlev ] the water level.
[vx] the u− component of velocity.
[vy] the v− component of velocity.
[tke ] the turbulent kinetic energy.
[epsilon ] the dissipation rate of turbulent kinetic energy.
ZERO Both the initial water level and velocity components are set to zero.
STEADY If this option is specified, the initial velocities will be derived from
the water levels using the Chezy formula for steady flow. This can
shorten the spin-up time of the SWASH run and can be meaningful
in the case of quasi-steady flow condition (e.g. flow in a river).](swashuse53x.svg)
| North |
| NW |
| West |
| SW | | -> CCW |
| -> SIDE < South > < > |
| | SE | | CLOCKWise | |
| | East | |
| | NE | |
| | | |
BOUndcond < | [k] | > &
| |
| |
| | -> XY < [x] [y] > | |
| | | |
| SEGMent < | < [i] [j] > | > |
| IJ < > |
| | < [k] > | |
BTYPe WLEV|VEL|DISCH|RIEMann|LRIEmann|WEAKrefl|SOMMerfeld|OUTFlow &
LAYer [k] | LOGarithmic &
SMOOthing [period] SEC|MIN|HR|DAY &
ADDBoundwave &
| FOURier [azero] < [ampl] [omega] [phase] >
| REGular [h] [per] [dir]
| BICHromatic [h1] [h2] [per1] [per2] [dir1] [dir2]
| CONstant < SPECTrum [h] [per] [dir] [dd] [cycle] SEC|MIN|HR|DAY
| | SERIes ’fname’ [itmopt]
| | SPECFile ’fname’ [cycle] SEC|MIN|HR|DAY
< &
| | FOURier < [len] [azero] < [ampl] [omega] [phase] > >
| | REGular < [len] [h] [per] [dir] >
| | BICHrom < [len] [h1] [h2] [per1] [per2] [dir1] [dir2] >
| VARiable < SPECTrum < [len] [h] [per] [dir] [dd] [cycle] S|MI|HR|DA >
| SERIes < [len] ’fname’ [itmopt] >
| SPECFile < [len] ’fname’ [cycle] SEC|MIN|HR|DAY >
| SPECSwan ’fname’ [cycle] SEC|MIN|HR|DAY
This command BOUNDCOND defines a boundary condition at the open boundary. It consists of two
parts, the first part defines the boundary side or segment where the boundary condition
will be imposed, the second part defines the type of the boundary condition and the
parameters.
There are two ways to define the part of the boundary at which the boundary condition is
imposed. The first way (SIDE) is easiest if the boundary is one full side of the computational
grid, although it should not be used for curved boundaries. The second method (SEGMENT) can be
used if the boundary segment goes around the corner of the grid, or if the segment is only part of
one side of the domain.
This BOUNDCOND command can be given a number of times, i.e. to define boundary conditions on
various sides or segments of the boundary. One BOUNDCOND command can be used for only one
side or one contiguous segment.
When no BOUNDCOND command is specified at a boundary, this boundary is considered to be a
closed one where the normal velocity at the boundary is set to zero.
Note that command BOUNDCOND can not be combined with the application of mass source
function for internal wave generation (see command SOURCE).
The specifications of the sub keywords are shown below. Please note that reference is made to the examples provided at the end of this section.
![SIDE the boundary is one full side of the computational grid (in 1D cases either
of the two ends of the 1D grid ).
NORTH, ... indicates on which side the boundary condition is applied. N means the
boundary is the north edge (if present) of the computational domain, likewise
for W is west, S is south, E is east, NW is northwest, NE is northeast,
SW is southwest and SE is southeast. Note that the boundary is assumed to
be a straight line. (Use the SEGMENT command as an alternative.)
Another note: in case of Cartesian coordinates, the direction of the problem
coordinate system must be defined by the user (see the SET ...[north ]
command ), by default the positive x− axis points East.
ONLY MEANT FOR STRUCTURED GRIDS.
[k] indicates on which side-of the unstructured-grid-the boundary condition is
applied. The value of [k] corresponds to the boundary marker as indicated in
file(s) produced by a grid generator (such as in the last column of the Triangle
.node file and the Easymesh .n file or the last part of file fort.14 ). Boundary
markers are tags to identify which vertices occur on a boundary of the mesh.
It is assumed that the full side in question is represented by a single
boundary marker.
ONLY MEANT FOR UNSTRUCTURED MESHES.
CCW, see description of [len] below; these option are only effective if the
CLOCKWISE option VARIABLE is used (see below ).
SEGMENT is used if SIDE is not used, i.e. either the boundary segment goes
around a corner of the grid, or the segment is only part of one side of the
grid. The distance along the segment (see [len ] below ) is measured
from the first point of the segment (see XY or IJ below ).
XY the segment is defined by means of a series of points in terms of problem
coordinates; these points do not have to coincide with grid points. The
(straight) line connecting two points must be close to grid lines of the
computational grid (the maximum distance is one hundredth of the length of
the straight line ).
This option is default.
[x], [y] problem coordinates of a point of the boundary segment (see command COORD ).
IJ the segment is defined by means of a series of computational grid points
given in terms of grid indices; not all grid points on the segment have to be
mentioned. If two points are on the same grid line, intermediate points are
assumed to be on the segment as well.
[i], [j] grid indices of a point of the segment. Values of [i] range from 1 to [mxc ]+1
and values of [j] from 1 and [myc ]+1 ([mxc] and [myc] as defined in the
command CGRID ).
ONLY MEANT FOR STRUCTURED GRIDS.
[k] index of boundary vertex of the segment. This can be obtained in a grid
generator file (.node and .n files of Triangle and Easymesh, respectively).
The order must be counterclockwise!
ONLY MEANT FOR UNSTRUCTURED MESHES.
BTYPE with this option the type of boundary condition is specified.
WLEV water level is imposed.
Required further specification by means of Fourier-series or time-series-
(see below ).
VEL velocity normal to the boundary is imposed.
Required further specification by means of Fourier-series or time-series-
(see below ).
DISCH discharge per unit width normal to the boundary is imposed.
Required further specification by means of Fourier-series or time-series-
(see below ). √ ---
RIEMANN Riemann invariant is imposed. It is de fined as u ± 2 gh with
u the velocity normal to the boundary and h the water depth.
The sign depends on the location of the boundary. The plus sign refers
to an inflow velocity at the western/left and southern/lower boundaries,
and the minus sign refers to inflow velocity at the eastern/right and
northern/upper boundary. This boundary condition is particularly meant
for a supercritical flow or hydraulic jump in e.g. rivers or open channels.
Required further specification by means of Fourier-series or time-series-
(see below ). ∘ ----
LRIEMANN linearized Riemann invariant is imposed. It is defined as u ± ζ g∕d
with u the velocity normal to the boundary, ζ the water level and d the
bottom level. The sign depends on the location of the boundary. The plus
sign refers to an inflow velocity at the western/left and southern/lower
boundaries, and the minus sign refers to inflow velocity at the eastern/right
and northern/upper boundary. Note that linearized Riemann invariants can
only be applied if the water level (ζ) is small compared to the local bottom
level (d). This is mainly applicable for a subcritical flow in relative deep
waters. Examples are tidal flows in a continental shelf or in a harbour.
Required further specification by means of Fourier series or time series
------------- -----------
(see below ).
WEAKREFL the boundary condition is weakly reflective.
Required further specification by means of Fourier-series or time-series-
of water level, or monochromatic,- bichromatic--or irregular waves by means
of a spectrum (see below). ---------------
SOMMERFELD Sommerfeld radiation condition is imposed. This condition is especially
useful for near-linear long waves at very shallow water.
No further specification is needed.
OUTFLOW water depth is aligned to bottom level (for supercritical river flow only
to obtain a so -called S2 backwater curve.)
No further specification is needed.
ONLY MEANT FOR STRUCTURED GRIDS.
LAYER indicates a layer where the boundary condition is imposed.
Only applicable to layer- dependent quantities.
[k] layer index (1 ≤ [k] ≤ [kmax] ).
LOGARITHMIC the vertical logarithmic profile for velocity at the boundary is assumed.
Only applicable to turbulent flows.
SMOOTHING with this option a ramp function is applied to the boundary condition in
order to start up the simulation smoothly.](swashuse59x.svg)
Further explanation and examples are given below. See also Section 5.3 for more details.
For each type of boundary condition (e.g., WLEV, VEL) a forcing type such as a Fourier series or a
time series must be prescribed. Exceptions to this are the commands SOMMERFELD and
OUTFLOW.
Instead of time-dependent forcing type (e.g., FOURIER, SERIES), a constant (in time) boundary value can be imposed. For instance, to impose a constant discharge of 2500 m3/s, give the following command
BOU ... BTYPE DISCHARGE CON 2500.
In case of velocity or discharge boundary condition the user may specify the vertical distribution
depending on the application. For turbulent flows, the user may specify the logarithmic velocity
distribution over the vertical at the open boundary. An alternative would be to specify the
velocity/discharge for each separate layer.
A uniform distribution over the vertical is assumed when none of the keywords LAYER [k] and
LOGARITHMIC is specified.
Note that by specifying regular or irregular waves at the open boundary using one of the
following commands REGULAR, BICHROMATIC, SPECTRUM or SPECFILE, the vertical profile of the
horizontal velocity derived from the first order Stokes wave theory is assumed. Hence, no type of
boundary condition (WLEV, VEL, etc.) nor vertical velocity profile should be specified. The
exception is specifying BTYPE WEAKREFL when a weakly reflective boundary is required. Also note
that the user can additionally specify the second order Stokes correction, if so desired (see
below).
Note that the forcing types FOURIER and SERIES are a generic one, which means they can be
used both for long waves (tidal waves, seiches, etc.) and short waves (monochromatic and
bichromatic waves or multiple Fourier modes). Therefore, in these cases, the user must explicitly
specify the type of the boundary condition (BTYPE ... including quantity) and the
vertical distribution of the velocity/discharge (LAYER [k] or LOGARITHMIC or none of
them).
At the wavemaker boundary, SWASH can accurately generate linear and nonlinear waves at any
depth using the derived solutions of the vertically discretized model equations based on the first
order and second order Stokes pertubation expansions. See Vasarmidis et al. (2024) for
a detailed explanation. This is, however, limited to up to four layers ([kmax] ≤ 4)
and they must be distributed equidistantly (see command VERT). In addition, the
Keller-box scheme for the non-hydrostatic pressure must be applied (see command
NONHYD BOX). If one of these three conditions is not fulfilled, then SWASH imposes the
vertical hyperbolic cosine velocity profile according to the linear wave theory (see also
Chapter 5).
First order monochromatic waves can be imposed using the command
BOU ... BTYPE WEAK ... CON REG ...
In this case the first order Stokes solutions of the surface elevation and the layer-averaged
velocities are imposed at the incident boundary. This also avoids the problem of the well-known
drop in the wave height in the first few grid points next to the boundary, especially for high
values of dimensionless depth kd. Note that weakly reflection at the open boundary
(keyword WEAK) is usually recommended in order to prevent re-reflections at the open
boundary.
Second order bound waves can be added by the following command
BOU ... BTYPE WEAK ... ADDBOUNDWAVE CON REG ...
By setting ADDBOUNDWAVE, self-interacting second order super-harmonics (doubled frequencies)
will be added to the first order Stokes waves. These super-harmonics are bound (phase-locked) to
the primary waves. Adding of these second order bound waves is required to suppress the
generation of spurious free modes, especially for high (nonlinear) waves. Since the added bound
waves are solutions to the discrete model equations, they exactly cancel the corresponding
spurious free waves at the wavemaker, thus leading to a spatially homogeneous wave field inside
the domain.
Bichromatic waves with periods 2π∕ωm and 2π∕ωn can be imposed at the open boundary similar to monochromatic waves. For instance, second order bichromatic waves can be prescribed where the interaction of two given components forces a second order bound wave group consisting of four components, namely, one sub-harmonic, ωm − ωn, and three super-harmonics, 2ωm, 2ωn and ωm + ωn. Specification of second order bichromatic waves is as follows
BOU ... BTYPE WEAK ... ADDB CON BICHromatic ...
With this command, six components will be imposed, two for the primary waves and four for
the bound waves. For the specification of only two primary wave components without
adding any other modes, remove ADDB or, alternatively, use the forcing type FOURIER
instead.
Irregular waves can also be generated at the open boundary using a weakly-reflective wavemaker based on one-dimensional or two-dimensional spectrum with a parametric shape, including second order bound waves (self-interacting super-harmonics and cross-interacting sub- and super-harmonics), as follows
BOU ... BTYPE WEAK ... ADDBoundwave CON SPECTrum ...
Instead of SPECTRUM the user can also define a 1D/2D non-parametric wave spectrum using
SPECFile or SPECSWAN.
Note that for the cases using unstructured meshes, only incident wave direction perpendicular to the open boundary is allowed.
| X | | | SOURce < -> Y > [centre] [width] [depth] [delta] & | | | [k] | | REGular [h] [per] [dir] < & | SPECTrum [h] [per] [dir] [dd] [cycle] SEC|MIN|HR|DAY SMOOthing [period] SEC|MIN|HR|DAY
This command SOURCE activates the generation of waves within the computational
domain using the spatially distributed mass source function. This command can not
be combined with the specification of boundary conditions at the boundaries (see
BOUNDCOND).
The user specifies a so-called source area, i.e. a rectangular area within the computational
domain, and subsequently a wave signal that will be generated in the source area. The
computational domain itself is assumed to be rectangular as well, however, the grid can
either be uniform or non-uniform. The user is advised to combine this internal wave
generation with sponge layers to absorb waves at boundaries effectively (see command
SPONGE).
The source area is a rectangle and is determined by means of its centroid (or the centre of
gravity) and its width. This rectangle is parallel either to the xc−axis or to the yc−axis of the
(rotated) rectilinear computational domain (see Figure 4.1), while its length extends along the
whole domain. In the first case the centroid is with respect to the xc−axis such that the
connecting line centroid−axis is parallel to the yc−axis, and the width is parallel to the yc−axis
as well. In the second case it is the other way around. In case of unstructured mesh,
the centroid is with respect to one side of the domain as specified by the boundary
marker.
The waves to be generated are either regular or irregular as defined by means of a wave
spectrum. First order Stokes (linear) wave theory is assumed. Note that a still water depth is
required (for the calculation of wave energy velocity).
Note that only incident wave direction perpendicular to the boundary is allowed in case of unstructured grids.
| North | | NW | | West | | SW | SPONgelayer < South > [width] | < [k] [width] > | SE | | East | | NE |
This command can be used to specify the sponge layers around the edges of the computational
domain.
Sponge layers are very effective in absorbing wave energy at open boundaries where waves are
supposed to leave the computational domain freely. So, they prevent reflections at open
boundaries. A sponge layer may have a width of 1 to 3 typical wave lengths.
Note that by including a sponge layer of [width] meters, the computational domain needs to be
extended with [width] meters as well (see command CGRID).
To specify the sponge layers, a distinction is made between structured and unstructured meshes.
The keywords NORTH, ... are meant for the structured grid only. Also note that the edge to
which a sponge layer is placed is assumed to be a straight line.
The variable [k] is to be used for the unstructured mesh (see below) and can be repeated as
many sponge layers to be chosen.
In case of Cartesian coordinates, the direction of the problem coordinate system must be defined by the user (see the SET ...[north] command), by default the positive x−axis points East.
FLOAT [alpha] [theta]
CANNOT BE USED IN CASE OF UNSTRUCTURED GRIDS.
With this optional command the user can specify some parameters in case of (fixed) floating objects or pressurized flow. See commands INPGRID DRAFT and READINP DRAFT in order to define floating objects. If these commands are not used, SWASH will not account for effects of floating structures on the (pressurized) flow.
BODY DIMension [l] [mass] [Ix] [Iy] [Iz] [cogx] [cogy] [cogz] & DOF SUrge SWay HEave ROll PItch YAw & ( MLIne < [K] [B] [apbx] [apby] [apbz] [apfx] [apfy] [apfz] [elen] > & PRETension ) & ( FENder < [K] [apfx] [apfy] [apfz] > )
CANNOT BE USED IN CASE OF UNSTRUCTURED GRIDS.
With this optional command the user can specify some dimensional parameters in case of moving rigid bodies. See commands INPGRID DRAFT and READINP DRAFT in order to define rigid bodies and also the commands INPGRID LABEL and READINP LABEL to label them (only necessary if more than one body is present). If these commands are not used, SWASH will not account for fluid-structure interactions.
| NEWmark [beta] [gamma] | | | | -> CH [rho] | BODY SOLVer < > COUPling [tol] [maxiter] [relax] & | HHT [rho] | | | | WBZ [rho] | KBC [theta]
CANNOT BE USED IN CASE OF UNSTRUCTURED GRIDS.
With this optional command the user can specify some numerical parameters for the rigid body
solver. The commands BODY DIMENSION and BODY SOLVER belong together.
A number of classical one-step implicit ODE solvers for the dynamic response systems are
available such as the Newmark’s method (1959) and the generalized−α method (Chung and
Hulbert, 1993). The method of Newmark is steered by two parameters 0 ≤ β ≤ 1∕2 and
0 ≤ γ ≤ 1 that control both accuracy and stability. The method is second order accurate if γ = 
and is unconditionally stable when 2β ≥ γ ≥
. However, γ > 
results in numerical damping.
Therefore, the common choice is β = 
and γ = 
, which is also known as the average
acceleration method.
The generalized−α method typically allows for numerical dissipation of high frequency noise
while minimizing unwanted low frequency dissipation. Examples are the Chung-Hulbert
(CH) scheme (1993), the Hilber-Hughes-Taylor (HHT) scheme (1977) and the
Wood-Bossak-Zienkiewicz (WBZ) scheme (1980), and are second order accurate and
unconditionally stable.
The parameter that counteracts the amplification of artificial high frequency modes is the
spectral radius of the amplification matrix, 0 ≤ ρ∞ ≤ 1. The highest amount of damping that
annihilates the highest frequency of interest in one time step is obtained by ρ∞ = 0, while a value
of one preserves the highest frequency mode. The CH scheme is known to be optimal in terms of
the amount of numerical damping.
The default time-marching method is the Chung-Hulbert scheme with ρ∞ = 1.
In order to predict the wave-induced response of a moored floating vessel (or a multiple WECs)
an iterative process is employed that tightly coupled the equations of rigid body motion to the
shallow water equations (including the non-hydrostatic pressure). Here, the motion of a rigid
body is a direct consequence of the wave-induced forces acting on it and, in turn, the fluid
surrounding the floating structure is influenced by the body movement (provided by the
kinematic boundary conditions at the fluid-structure interface). The approach is to solve each
subsystem independently (fluid flow and body motion, respectively), and subsequently implicitly
coupled in an iterative Gauss-Seidel type manner. Convergence is reached when changes
to the body motions within the iterative procedure are smaller than a user-defined
tolerance. By default this is 10−4, whereas the maximum number of iterations is set to
50.
It is well known that fluid-structure coupling algorithms tend to become unstable in case of light bodies that are subjected to high acceleration. A common approach to improve the convergence rate of such iteration schemes is to apply under-relaxation. The optimal value of the under-relaxation coefficient, as indicated here by [relax], is problem-dependent, in particular, in the context of nonlinear problems. However, here we proposed a fixed low value of 0.3, which seems to be reasonable for moored floating structures.
![NEWMARK this option indicates that the Newmark scheme will be adopted.
[beta ] the first Newmark time integration parameter.
Note: 0 ≤ [beta] ≤ 0.5.
Default: [beta ] = 0.25
[gamma ] the second Newmark time integration parameter.
Note: 0 ≤ [gamma ] ≤ 1.
Default: [gamma ] = 0.5
CH this option indicates that the Chung -Hulbert scheme will be adopted.
This is the default.
HHT this option indicates that the Hilber -Hughes -Taylor scheme will be adopted.
WBZ this option indicates that the Wood -Bossak -Zienkiewicz scheme scheme will
be adopted.
[rho ] parameter that controls the spectral distribution of numerical dissipation.
Note: 0 ≤ [rho] ≤ 1.
Default: [rho ] = 1.0.
COUPLING with this option the user can determine parameters for the fluid -structure
coupling.
[tol ] error tolerance to terminate the iteration process.
Default: [tol ] = 0.0001.
[maxiter ] maximum number of iterations.
Default: [maxiter ] = 50.
[relax ] the under-relaxation coefficient.
Note: 0 ≤ [relax ] ≤ 1.
Default: [relax ] = 0.3.
KBC with this option the user can determine the parameter below for the
kinematic boundary conditions at fluid-structure interface.
[theta ] the weighting parameter to determine the body velocities (both
translational and rotational) at an intermediate time between previous
and current time step.
Note: 0 ≤ [theta ] ≤ 1, with [theta ] = 0 corresponding to the previous
value and [theta ] = 1 to the current value.
Default: [theta ] = 0.5](swashuse79x.svg)
| -> CONstant [cd] | | | | CHARNock [beta] [height] | | | | LINear [a1] [a2] [b] [wlow] [whigh] | | | | REL [alpha] WIND [vel] [dir] < WU > < | | | RELW [crest] | GARRatt | | | | SMIthbanke | | | | FIT |
With this optional command the user can specify wind speed, direction and wind drag. Wind
speed and direction are assumed constant. If this command is not used, SWASH will not account
for wind effect.
This command is usually meant for large-scale wind driven circulation, tides and storm surges.
Inclusion of wind effects may also be beneficial to buoyancy driven flows in coastal seas, estuaries
and lakes. However, this option may also be useful for applications concerning wind effects on
wave transformation in coastal waters, ports and harbours.
In SWASH seven different wind drag formulation are available, i.e., constant, linear on wind
speed, Charnock, Wu, Garratt, Smith and Banke and the second order polynomial fit. The
Charnock drag formulation is based on an implicit relationship between the wind and the
roughness, while the other formulations, those of Wu, Garratt and Smith and Banke, express a
linear relationship between the drag and the wind speed.
Recent observations indicate that these linear parameterizations overestimate the drag coefficient at high wind speeds (U10 > 20 m/s, say). Based on many authoritative studies it appears that the drag coefficient increases almost linearly with wind speed up to approximately 20 m/s, then levels off and decreases again at about 35 m/s to rather low values at 60 m/s wind speed. We fitted a 2nd order polynomial to the data obtained from these studies, and this fit is given by
where Ũ = U10∕Uref, and the reference wind speed Uref = 31.5 m/s is the speed at which the
drag attains its maximum value in this expression. These drag values are lower than in the
expression of Wu (1982) by 10% − 30% for high wind speeds (15 ≤ U10 ≤ 30 m/s) and over 30%
for hurricane wind speeds (U10 > 30 m/s).
Usually, the wind stress depends on the drag and the wind speed at a height of 10 m, U10.
However, it might be obvious that the influence of wind stress will reduce if the water is flowing
in the same direction and it will decrease when the water flow and wind are in opposite
directions. This may lead to a smaller wind setup on very shallow areas. Hence, the wind stress
may be dependent on the wind velocity relative to the water, i.e. U10 − u, instead of
the wind velocity as such. Here, u is either the depth-averaged flow velocity in the
depth-averaged mode or the surface flow velocity in the multi-layered mode. Experiments
have shown that the eigenfrequencies damp out much faster when this alternative is
employed.
The considered wind is at 10 m above the surface. However, it might be better to consider the
wind at the surface in order to relate this wind to the flow velocity. A factor α (0 < α ≤ 1) is
introduced that take into account the difference between the wind velocity at 10 m height and
the wind velocity at the surface, Us = αU10. With the use of α in this formulation the influence
of the flow velocity becomes even stronger. However, the exact value of α is yet unknown; further
research on this parameter is needed. Therefore, this parameter is optionally and should be used
with care.
Wave growth due to wind in shallow areas is included in the model. It is based on a parameterization of the momentum flux transferred from wind to surface waves similar to the well-known sheltering mechanism of Jeffreys (1925) as described in Chen et al. (J. Waterwy, Port, Coastal, Ocean Engng., 130, 312-321, 2004). The wind stress is expressed by
where ρair is the air density and c is the wave celerity. Hence, the wind velocity is
taken relative to the wave celerity. The wind stress may vary over a wave length with
a larger wind drag on the wave crest than that in the trough (Chen et al., 2004).
This effect is implemented in the model by applying the wind stress on the wave crest
only.
The default option is a constant wind drag coefficient, while the wind stress is related to the wind velocity at 10 m height only.
![[vel ] wind velocity at 10 m height (in m/s ).
[dir ] wind direction at 10 m height (in degrees; Cartesian or Nautical
convention, see command SET).
CONSTANT this option indicates that a constant drag coefficient will be adopted.
[cd] dimensionless coefficient.
Default: [cd] = 0.002
CHARNOCK indicates that the Charnock drag formulation will be adopted.
[beta ] dimensionless Charnock coefficient.
Default: [beta ] = 0.032
[height ] height (in m ) above the free surface where the wind speed has been measured.
Default: [height ] = 10.
LINEAR indicates that the wind drag depends linearly on wind speed.
For this, both lower and upper bounds of the wind speed, [wlow ], [whigh ],
and two coefficients, [a1], [b], need to be specified as follows:
cd = 0.001( [a1 ] + [b] U10), with cd the drag coefficient and U10 the wind
speed in between [wlow ] and [whigh ].
[a1] coefficient in the above linear function.
[a2] not used.
[b] coefficient in the above linear function.
[wlow ] lower bound of wind speed.
[whigh ] upper bound of wind speed.
WU indicates that the drag formulation of Wu will be adopted.
GARRATT indicates that the drag formulation of Garratt will be adopted.
SMITHBANKE indicates that the drag formulation of Smith and Banke will be adopted.
FIT drag coefficient is based on the 2nd order polynomial fit.
RELATIVE indicates that the wind stress depends on the wind velocity relative to the water.
[alpha ] parameter to relate the wind velocity at 10 m height to wind velocity at surface.
Note: 0 < [alpha ] ≤ 1.
Default: [alpha ] = 1.
RELWAVE indicates that the wind stress depends on the wind velocity relative to the
wave celerity. This option enables to include wind effects on the nearshore
wave transformation.
[crest ] free parameter representing a ratio of the forced crest height to maximum
surface elevation. Use of this parameter implies that the wind stress is only
applied on wave crests of which the surface elevation is larger than the given
fraction [crest ] of the maximum elevation with respect to the datum level.
Note: 0 ≤ [crest ] ≤ 1.
Default: [crest ] = 0.4](swashuse84x.svg)
The quantities [vel] and [dir] are required if this command is used except when the command
READINP WIND is specified.
| CONstant [cf] | | CHEZy [cf] | | -> MANNing [cf] FRICtion < | COLEbrook [h] | | | -> SMOOTH | LOGlaw < | ROUGHness [h]
With this optional command the user can activate bottom friction. If this command is not used,
SWASH will not account for bottom friction.
For typically depth-averaged calculations, four different bottom friction values are available, i.e.,
constant, Chezy, Manning and Colebrook-White values. Note that the Colebrook-White friction
value equals the Nikuradse roughness height. Although they are associated with depth-averaged
flow velocities, they may be applied in the multi-layered mode as well. However, some
inaccuracies may occur in the vertical structure of the velocity, in particular when the
depth-averaged velocity is zero. Alternatively, the logarithmic wall law may be applied. In this
case, a distinction is made between smooth and rough beds. For rough beds, the user must apply
a Nikuradse roughness height.
The aforementioned friction formulations are usually derived for quasi-steady flow condition (e.g.
flow in a river). However, numerical experiments have indicated that the Manning formula
provides a good representation of wave dynamics in the surf zone, and even better to that
returned by other friction formulations.
The default option is: MANNING with a constant friction coefficient.
| -> CONstant [visc] | | -> Horizontal < SMAGorinsky [cs] | | | | MIXing [lm] | | VISCosity < Vertical KEPS [cfk] [cfe] | | | | -> LINear | FULL KEPS < | | NONLinear
With this optional command the user can activate turbulent mixing. If this command is not
used, SWASH will not account for turbulent mixing.
The turbulence structure of the flow in shallow water is characterized by the coexistence of
three-dimensional turbulence, having length scales less than the water depth, and horizontal
two-dimensional eddies with much larger length scales. Such a non-isotropic character of shallow
water turbulence may produce a large difference between horizontal and vertical eddy viscosity
coefficients.
Three-dimensional turbulence is mainly generated by vertical velocity gradients (including
bottom and wind stresses) whose length scale is smaller than the water depth. Therefore, a
turbulence model is necessary to properly evaluate the vertical momentum exchange in
flows. This is represented by the vertical eddy viscosity coefficient in the momentum
equations.
In estuaries and coastal seas the large-scale flow patterns are usually determined by tidal forcing,
the baroclinic pressure gradient, wind and bottom friction, whereas the horizontal turbulent
stresses have little impact. Hence, for far field calculations the use of an horizontal eddy viscosity
model has a negligible role. On the other hand, for near field flows, horizontal large-scale
eddies generated by lateral shear may have a significant role in horizontal mixing.
Examples are mixing layers developing at harbour entrances, along groyne fields and
floodplains, separation flows, wakes and jets, and flows near discharges. The horizontal
exchange of turbulent momentum need to be modelled properly, since a constant value
for the horizontal eddy viscosity is too crude as an assumption for such near field
predictions.
In SWASH both the horizontal and vertical eddy viscosities can be specified, either
separately or combined. In such cases, the pressure is assumed to be hydrostatic. In
addition, the Boussinesq hypothesis is applied that basically assumes the isotropy of
turbulence.
Three different horizontal eddy viscosity models are available, i.e., a constant viscosity, the
Smagorinsky model and the Prandtl mixing length hypothesis. Vertical mixing can be modelled
by using the standard k − 𝜀 model, with k the turbulent kinetic energy per unit mass and 𝜀 the
dissipation rate of turbulent kinetic energy per unit mass (Launder and Spalding,
1974).
Within the vegetation canopy, it is assumed that all energy of the mean flow is converted to
turbulent energy due to the plant drag (see command VEGETATION). This process is
modelled by means of the vegetation-induced turbulence production terms in the k − 𝜀
model. They are accompanied with two empirical constants [cfk] and [cfe] associated
with k and 𝜀, respectively. We have selected the values as suggested by Shimizu and
Tsujimoto (1994), i.e. [cfk] = 0.07 and [cfe] = 0.16 (see also Defina and Bixio,
2005).
SWASH offers the user the possibility to simulate a full three-dimensional turbulent flow where
both non-hydrostatic pressure and anisotropic state of turbulent stresses becomes important.
Additionally, the length scales in all directions can be in the same order. Examples are curved
open channel flows with heterogeneous roughness conditions and compound channel
flows with different floodplains. Their flow characteristics are represented by, amongst
others, secondary currents (of Prandtl’s second kind) generated due to anisotropy of
turbulence.
For such cases a three-dimensional turbulence model should be activated, where the Reynolds
stresses in all directions are equally important. These turbulent stresses are supposed to be
linearly related to the deformation rates of the mean flow. This Boussinesq hypothesis introduces
the concept of eddy viscosity that can be computed by means of a two-equation model. The
standard k −𝜀 model of Launder and Spalding (1974) is employed, whereas the eddy viscosity is
applied to all directions. The Boussinesq hypothesis can be considered as the leading term in a
series expansion of products of strain and rotation tensors implying isotropy of turbulence. This
works quite well for many flows where the primary shear stress is the dominant one. This
is, however, not the case when secondary shear stresses and normal stresses become
relevant. Hence, the Boussinesq hypothesis may not be suitable for turbulent flows
involving strong three-dimensional effects. This weakness can potentially be removed by
expanding the stress-strain relationship to include the quadratic terms of the mean velocity
gradient tensor. These terms approximate the deviations from the isotropic state of the
turbulent normal stresses. To this end, the nonlinear k − 𝜀 model of Speziale (1987) is
applied.
The default option is a constant horizontal eddy viscosity.
POROsity [size] [height] [alpha0] [beta0] [wper]
CANNOT BE USED IN CASE OF UNSTRUCTURED GRIDS.
This command indicates the use of porosity layers inside the computational domain
to simulate full/partial reflection and transmission through porous structures such
as breakwaters, quays and jetties. Also the interaction between waves and porous
coastal structures can be simulated in this way. The mean flow through porous medium
is described by the volume-averaged Reynolds-averaged Navier-Stokes (VARANS)
equations. The laminar and turbulent frictional forces in porous medium is modelled by
means of the empirical formula’s of Van Gent (1995). In the case of an oscillatory wave
motion the turbulent loss will enhance, which depends on the Keulegan-Carpenter
number.
See commands INPGRID POROSITY and READINP POROSITY in order to define porosity layers. If neither of this command nor the command READINP POROSITY is used, SWASH will not account for wave interactions with porous structures.
VEGEtation < [height] [diamtr] [nstems] [drag] > INERtia [cm] POROsity Vertical
CANNOT BE USED IN CASE OF UNSTRUCTURED GRIDS.
With this optional command the user can activate wave damping induced by aquatic vegetation.
If this command is not used, SWASH will not account for vegetation effects.
The vegetation (rigid plants) can be divided over a number of vertical segments and so, the
possibility to vary the vegetation vertically is included. Each vertical segment represents some
characteristics of the plants. These variables as indicated below can be repeated as many vertical
segments to be chosen.
The vegetation effect is due to the drag force on a fixed body in an oscillatory flow
which can be determined using the well-known Morison equation. In this case only
vertical cylinders are considered and the direction of the drag force is horizontal. Apart
from the drag force, the inertia force can be optionally included, which is specified
by means of the added mass coefficient. Note that this coefficient is one less than
the inertia coefficient (=Froude-Krylov force + added mass) and is uniform over the
plant.
For the case of densely spaced cylinders, like dense mangrove fields and porous brushwood groins,
the effect of porosity can be optionally included. This porosity depends on the spatial occupation
of vegetation per unit volume.
In case horizontal cylinders are included (e.g. box filled with branches or mangrove with both horizontal and vertical roots), the drag forces in both the horizontal and vertical directions must be modelled.
| -> Sec | | -> NONCohesive [size] | TRANSPort [diff] [retur] < MIn > < > & | HR | | COHesive [tauce] [taucd] [erate] | | DAy | | -> Yes | [fall] [snum] [ak] DENSity < > | No | ANTICreep None | STAndard | SVK
With this optional command the user can specify some relevant parameters in case of transport
of constituent. These parameters are only relevant when transport of salinity, temperature, or
suspended sediment load is included.
Inclusion of transport of constituent is indicated by the commands INPTRANS SALINITY and
READTRANS SALINITY in case of salinity, or the commands INPTRANS TEMPERATURE and
READTRANS TEMPERATURE in case of temperature, or the commands INPTRANS SEDIMENT and
READTRANS SEDIMENT in case of suspended sediment load. Using these commands, both the
initial and stationary boundary conditions for constituent are thus specified. If none
of these commands is used, SWASH will not account for transport of any of these
constituents.
The first parameter that may be specified in this command is the horizontal eddy diffusivity. A
uniform eddy diffusivity value may be chosen that can be used as a calibration parameter to
account for all forms of unresolved horizontal mixing. This parameter may be chosen
independently from the eddy viscosity (see command VISCOSITY HOR). The eddy diffusivity
depends on the flow and the grid size used in the simulation. A typical small-scale model with
grid sizes of tens of meters or less, the eddy diffusivity typically ranges from 1 to 10
m2/s. For a large-scale (tidal) areas with grid sizes of at least hundreds of meters,
the parameter is typically in the range of 10 to 100 m2/s. Alternatively, when not
specified, the eddy diffusivity is related to the eddy viscosity that is determined by
either the Smagorinsky model or the Prandtl mixing length model. Otherwise it is
zero.
Note that in 3D simulations the vertical eddy diffusivity is automatically included and is related
to the vertical mixing (see command VISCOSITY VERT).
The second parameter in this command is the return time for unsteady salt intrusion in a tidal flow. A boundary condition at the seaward side is required. This is usually the ambient or background concentration of salt sea water. However, at the transition between sea and river, alternating conditions hold regarding inflow of salt sea water during flood tide and outflow of fresh river water during ebb tide. Immediately after low water, the salinity of the inflowing water will not be equal to the salinity of the sea water. It will take some time before this happens at the boundary. This time lag is the return time for salinity from its value at the outflow depending on conditions in the interior of model domain relative to its background value specified at the inflow, see Figure 4.2.
This memory effect is characterised by the so-called Thatcher-Harleman condition that
specifies an appropriate time lag. The return time depends on the tidal flow conditions outside
the estuary.
Either noncohesive suspended sediment (sand) or cohesive suspended sediment (mud or clay) transport can be considered. We assume a single sediment class. Bed load is not taken into account. In case of noncohesive suspended load transport, median sediment diameter can be specified. In this respect, a pickup function is employed to model the upward sediment flux in which the amount of noncohesive sediment (sand) is eroded from the bed surface into the flow. The following pickup function is used (Van Rijn, 1984):
with c the (volumetric) sediment concentration, νt the vertical eddy viscosity (see command VISCOSITY VERT), σc the Schmidt number for sediment, 𝜃 the Shields parameter related to the bed shear stress, 𝜃cr = 0.05 the critical Shields parameter, s = 2.65 the sediment specific gravity (see command SET [rhosed]), d50 the median sediment diameter, and ν the kinematic viscosity of water. Sediment deposition is determined by the downward flux related to the settling velocity ws. If this fall velocity is not specified by the user, then the fall velocity will be calculated by SWASH depending on the particle size (Rubey, 1933):
Note that if the sediment diameter is not specified by the user, then no mass exchange between
the bed and the flow will be taken into account.
For cohesive sediment the mass exchange of suspended load between the bed and the flow are calculated with the well-known Partheniades-Krone formulations, which include the erosion and deposition fluxes:
The sediment flux for erosion is given by
where E is the entrainment rate for erosion flux, τce is the critical bed shear stress for erosion and τb is the actual bed shear stress. The sediment flux for deposition is given by
where cb is the (volumetric) sediment concentration near the bed and τcd is the critical bed
shear stress for sedimentation. Here, the critical bed shear stresses for erosion, τce, and
sedimentation, τcd, the sediment erosion rate E and the fall velocity ws must be specified by the
user.
It is assumed that the interaction between sediment and turbulent flow is mainly governed by
sediment-induced buoyancy effects. In this respect, the standard k − 𝜀 model and the
logarithmic wall law near the bed surface must be applied. This wall law is used to
calculate the bed shear stress τb, which in turn serves as one of the parameters for the
mass exchange between the bed and the flow. For sand transport the roughness height
may depend on the sediment diameter (if the user wants so) and is determined as
5.5 d50.
Because of the assumption of the upward sediment flux being equal to the pickup rate, the
Schmidt number σc for sediment becomes a free parameter. Experiences have shown that
sediment diffusivity is rather sensitive to this parameter. The sediment diffusivity is usually
larger than the eddy viscosity, and so σc < 1.
The turbidity flow is usually considered as a mixture of water and sediment with a mixture
density, i.e. the effect of sediment on the density of (salt) water is included. However, in some
cases it may be desirable not to include this effect. In this case the density of water remains
unchanged, while the sediment transport is only influenced by the flow and (turbulent)
dispersion. Also, there is no sedimentation and erosion near the bed. Hence, sediment can be
considered here as a passive tracer.
SWASH makes use of the terrain-following coordinates of which the advantages are a better representation of bottom topography and a better resolution in shallow areas. A disadvantage is the transformation of the transport equation due to the geometrical properties of the curved z-planes, so that the curvature terms are involved, which may complicate the computation. However, when these curvature terms are neglected, this may lead to a false generation of vertical mixing. This effect, known as the artificial creeping, becomes evident when the bottom slope is relatively large in regions of strong stable stratification. Hence, in such as case, inclusion of the curvature terms, known as the anti-creepage terms, may reduce significantly the artificial creeping. The standard method is based on the actual transformation. An alternative is the method of Stelling and Van Kester [3], which computes the horizontal diffusion along strictly horizontal planes.
BREaking [alpha] [beta]
With this optional command the user can control depth-limited wave breaking in the case of
relatively coarse resolution in the vertical. If this command is not used, SWASH will not account
for this control. Note that SWASH will account for energy dissipation due to wave breaking
anyhow. Also note that the use of this command in the case of current-limited wave breaking (see
command AMBIENT) is strongly discouraged.
By considering the similarity between breaking waves and bores or moving hydraulic jumps, energy dissipation due to wave breaking is inherently accounted for. However, when a few vertical layers are to be employed, the amount of this energy dissipation may be underestimated due to the inaccuracy with which the phase velocity at the front face of the breaking wave is approximated. To initiate the wave breaking process correctly, steep bore-like wave fronts need to be tracked and this can be controlled by the vertical speed of the free surface. When this exceeds a fraction of the shallow water celerity, as follows,
the non-hydrostatic pressure in corresponding grid points is then neglected and remains so at
the front face of the breaker. The parameter α > 0 represents the maximum local surface
steepness and determines the onset of the breaking process. A threshold value of α = 0.6 is
advised. (This corresponds to a local front slope of 25o.) This single value is not subject to
calibration and seems to work well for all the test cases we have considered, both regular and
irregular waves.
To represent persistence of wave breaking (even if ∂tζ < α
), we also label a grid point for
hydrostatic computation if a neighbouring grid point has been labelled for hydrostatic
computation and the local steepness is still high enough, i.e.,
with β < α. In all other grid points, the computations are non-hydrostatic.
This approach combined with a proper momentum conservation leads to a correct amount of
energy dissipation on the front face of the breaking wave. Moreover, nonlinear wave properties
such as asymmetry and skewness are preserved as well.
Note that by taking a sufficient number of vertical layers (10 or so) the phase velocity at the breaking front will be computed accurately enough and hence, this option should not be activated.
AMBient [U] [V] [eta]
CANNOT BE USED IN CASE OF UNSTRUCTURED GRIDS.
With this optional command the user can specify spatially constant ambient current and mean water level to include their effect on waves. If this command is not used, SWASH will not account for the effect of ambient current on the wave dynamics unless the commands INPAMB and READAMB are activated.
![[U] the x− component of the ambient current (in m/s).
Note that [U ] is allowed to vary over the computational region; in that
case use the commands INPAMB AXV and READAMB ACURR to define and
read the associated data. The value of [U ] in this command will be
ignored.
[V] the y− component of the ambient current (in m/s).
Note that [V ] is allowed to vary over the computational region; in that
case use the commands INPAMB AVY and READAMB ACURR to define and
read the associated data. The value of [V ] in this command will be
ignored.
[eta ] the mean water level (in m).
Note that [eta ] is allowed to vary over the computational region; in that
case use the commands INPAMB MWL and READAMB MWL to define and
read the associated data. The value of [eta ] in this command will be
ignored.](swashuse113x.svg)
NONHYDrostatic / STAndard \ [theta] & \ -> BOX / SUBGrid [pmax] REDuced [qlay] & SOLVer [rhsaccur] [initaccur] [maxiter] [relax] & PREConditioner ILUD|ILU & PROJection ITERative [tol] [maxiter]
With this optional command the user can include the non-hydrostatic pressure in the shallow
water equations. If this command is not used, SWASH will not account for non-hydrostatic
pressure, i.e. pressure is assumed to be hydrostatic.
Hydrostatic pressure assumption can be made in case of propagation of long waves, such as
large-scale ocean circulations, tides and storm surges. This assumption does not hold in case of
propagation of short waves, flows over a steep bottom, unstable stratified flows, and other
small-scale applications where vertical acceleration is dominant.
In SWASH two different schemes for the vertical pressure gradient are available, i.e., the classical
central differencing (option STANDARD) and the Keller-box scheme (option BOX). The former
approximation is particularly meant for applications where vertical structures are important, e.g.
stratified flows with density currents, undertow and flows over steep and rapidly varying
bottoms, while the latter will be mainly used for accurate short wave propagation with two or
three layers employed. In addition, when applying the Keller-box scheme, it is advised to
choose an equidistant layer distribution (variable thicknesses only) in order to get
the optimal linear frequency dispersion accuracy (i.e. the relative error of the phase
speed predicted by the model compared to that from the linear dispersion theory is
minimal).
The time integration of the vertical pressure gradient is the so-called 𝜃−scheme (a mix of explicit
and implicit Euler schemes). With [theta] = 0.5 we have the well-known second order accurate
Crank-Nicolson scheme with the smallest truncation error, while [theta] = 1 indicates the first
order implicit Euler scheme. Note that only values of [theta] in the range [0.5,1] are allowed for
stability reasons.
The number of vertical layers is chosen sufficiently large to resolve the vertical structure of the
flow field (see command VERTICAL). However, this grid resolution in the vertical is also employed
in the discretization of the non-hydrostatic pressure field, whereas a few number of layers usually
suffices to compute wave dispersion without deteriorating accuracy. With a subgrid approach the
user has an option to resolve the flow and pressure field with a different resolution in the vertical.
The vertical is equidistantly divided into a few number of layers for the non-hydrostatic
pressure and a relative large number of (non-equidistant) layers for the horizontal
velocities and turbulent stresses. In this way, the solution for the non-hydrostatic pressure
and vertical acceleration can be obtained on a relatively coarse vertical grid, while
on a subgrid with a high vertical resolution the vertical structure of turbulent flow
is resolved. Note this subgrid approach cannot be applied in the case of pressurized
flow.
Since most of the computational effort is devoted to inverting the Poisson pressure matrix, an
effective way to minimize this effort is by reducing the rank of the Poisson matrix. This leads to
less computational cost and memory. With the keyword REDUCED the dimension of the Poisson
equation, i.e. the number of pressure unknowns per water column, can be diminished. Note this
option must be combined with the BOX scheme. In spite of this reduction it can still provide an
accurate description of dispersive waves. For instance, a model with two layers but one reduced
pressure layer, the so-called reduced two-layer model, has more or less the same linear dispersion
accuracy as the full two-layer model but saves about 30% CPU time. Note this option cannot
be applied in the case of pressurized flow. The stencil of the pressure equation can
be reduced by assuming a constant pressure in the vertical near the bottom. This is
determined by the parameter [qlay] which indicates the number of layers, started from the
bottom, where the pressure is constant. In this way, it is possible to eliminate the
pressure in these layers from the set of equations. As an example, we have a model
with five pressure layers ([pmax] = 5) and we assume that the pressure is constant in
the two lowest layers ([qlay] = 2). So there are effectively three (upper) layers in
which the pressure need to be computed. An important remark needs to be made.
Although this reduced pressure equation method is more efficient in terms of CPU time,
it is less so concerning the dispersion accuracy. To optimize this accuracy often a
different than equidistant layer distribution needs to be sought. For instance, the optimal
linear dispersion relation of the reduced two-layer model ([kmax] = [pmax] = 2,
[qlay] = 1) is obtained by setting the following layer distribution: the top layer has a
relative thickness of 84% whereas the thickness of the bottom layer is 16% of the total
depth.
By inclusion of the non-hydrostatic pressure, a solution of the Poisson pressure equation is
required. In SWASH this equation is solved by an iterative solution method and the user
may controls this by means of the keyword SOLVER. Two linear solvers are adopted:
Strongly Implicit Procedure (SIP) and BiCGSTAB preconditioned with an incomplete
LU factorization. The former one is particularly meant for the depth-averaged case,
while the latter one is to be applied for the multi-layered case. The incomplete LU
factorization is either ILU or ILUD. The latter is restricted to the main diagonal of
the matrix, i.e. the off-diagonals remain unchanged. The choice of the preconditioner
is indicated with the keyword PRECONDITIONER. For parallel computing, the ILUD
preconditioner is a good choice. However, the ILU preconditioner is more robust. For instance,
when high waves or very short waves are involved, or when the bottom topography
exhibits steep slopes, or when a considerable number of layers (> 20) is involved, it
may be wise to choose the ILU preconditioner. Note this ILU preconditioner will be
chosen automatically in the case of pressurized flow and/or unstructured triangular
meshes. The weighting parameter α, as indicated by [relax], may improve the rate of
convergence. With this parameter a combination of the classical ILU and the modified
ILU (MILU) can be given. This combination is given by (1-α)ILU + αMILU, and is
also hold for ILUD and its modified variant (MILUD). Based on several numerical
experiments, an optimum in the convergence rate is found by taking 55% of MILU and 45%
of ILU in case of the Keller-box scheme, and 99% of MILUD and 1% ILUD for the
same scheme, while for the standard discretization of the vertical pressure gradient, a
combination of 90% of MILU(D) and 10% of ILU(D) is chosen. Note that in the case of
unstructured triangular meshes, the default value is the ILU preconditioner (thus 0%
MILU).
It is common to use the reduction of the residual as a stopping criterion, because the BiCGSTAB
method requires calculation of the residual. When solving the system Ax = b, after m iterations
we have an approximate solution xm and the residual rm = b − Axm is related to the
convergence error em = x − xm by Aem = rm, so the reduction of the residual results
in the reduction of the convergence error. This does not necessarily mean that the
relative error of the solver is identical to the decrease of the residual. The iteration
process stops at each time step if the ratio of the 2-norm of the residual and of the
right-hand side or initial residual is less than a given accuracy: ∥rm∥2∕∥b∥2 < 𝜖 and
∥rm∥2∕∥r0∥2 < 𝜖, respectively. They are indicated by the parameters [rhsaccur] and
[initaccur], respectively. If both these accuracies are given, the sum of the two is used as
termination criterion. Often, the stopping criterion for the iterative methods is basically a
compromise between efficiency and accuracy. Decreasing the required accuracy can save a
considerable amount of CPU time. Numerical experiments showed 𝜖 = 0.01 gives the
optimum.
The Poisson pressure equation is obtained by means of the pressure correction method of Van
Kan (1986). This method is second order accurate in time and thus appropriate for the
simulation of wave transformation, or in general, free surface flows. To deal with the pressurized
flow underneath a floating object, the user is advised to choose the first order pressure projection
method of Chorin (1968). However, to retain the second order accuracy and to avoid wave
damping when simulating free surface flows, the accuracy of the pressure projection method can
be improved. This is accompanied by an iteration process to solve the global continuity equation
containing the contribution of the non-hydrostatic pressure. This equation is then consistent with
the divergence-free velocity field obtained after the pressure projection step (Vitousek and
Fringer, 2013).
The default option is the Keller-box scheme with [theta] = 1.0, while the Poisson pressure equation obtained with the second order pressure correction technique is solved with either SIP with [rhsaccur]=0.01, in the case of depth-averaged mode, or ILUD-BiCGSTAB with [rhsaccur]=0.01 and [initaccur]=0, in the case of multi-layered mode. For unstructured meshes, the ILU-BiCGSTAB solver is chosen instead.
![X source area is parallel to xc− axis of the rectilinear grid.
Y source area is parallel to yc− axis of the rectilinear grid.
This is default.
[k] indicates from which side of the unstructured grid [centre ] is measured.
---- ------------------
The value of [k] corresponds to the boundary marker as indicated in file(s)
produced by a grid generator (such as in the last column of the Triangle
.node file and the Easymesh .n file or the last part of file fort.14 ). Boundary
markers are tags to identify which vertices occur on a boundary of the mesh.
It is assumed that the full side in question is represented by a single
boundary marker.
ONLY MEANT FOR UNSTRUCTURED MESHES.
[centre ] the centre of gravity of source area in meters.
[width ] the width of source area in meters.
[depth ] the still water depth at source area in meters.
[delta ] shape parameter for the source function.
Default: [delta ] = 0.5
REGULAR regular waves will be generated. See command BOUNDCOND for the
specification of their parameters.
SPECTRUM irregular waves will be generated. See command BOUNDCOND for the
specification of their parameters. See also command BOUND SHAPE
for spectral shape.
SMOOTHING with this option a ramp function is applied to start up the simulation smoothly.
[period ] the smoothing period of which the unit is indicated in the next option:
SEC unit seconds
MIN unit minutes
HR unit hours
DAY unit days](swashuse62x.svg)
![NORTH sponge layer is placed at the north edge of the domain.
NW sponge layer is placed at the northwest edge of the (rotated) domain.
WEST sponge layer is placed at the west edge of the domain.
SW sponge layer is placed at the southwest edge of the (rotated) domain.
SOUTH sponge layer is placed at the south edge of the domain.
SE sponge layer is placed at the southeast edge of the (rotated) domain.
EAST sponge layer is placed at the east edge of the domain.
NE sponge layer is placed at the northeast edge of the (rotated) domain.
ONLY MEANT FOR STRUCTURED GRIDS.
[k] indicates on which side-of the unstructured-grid-the sponge layer is applied.
The value of [k] corresponds to the boundary marker as indicated in file(s)
produced by a grid generator (such as in the last column of the Triangle
.node file and the Easymesh .n file or the last part of file fort.14 ). Boundary
markers are tags to identify which vertices occur on a boundary of the mesh.
It is assumed that the full side in question is represented by a single
boundary marker.
ONLY MEANT FOR UNSTRUCTURED MESHES.
[width ] the width of sponge layer in meters.](swashuse65x.svg)
![[alpha ] compressibility factor for flow beneath fixed floating object.
This option is meant for academic purposes only.
Note: 0 ≤ [alpha ] ≤ 1.
Default: [alpha ] = 0.
[theta ] parameter for the 𝜃− method applied beneath floating object.
[theta ] = 0.5 corresponds to the Crank -Nicolson scheme and
[theta ] = 1 to the implicit Euler scheme.
Default: [theta ] = 1.](swashuse68x.svg)
![[l] the label number for each rigid body.
This number must correspond to that of the label as specified by
the commands INPGRID LABEL and READINP LABEL.
[mass ] body mass (in kg).
2
[Ix] moment of inertia of body around the x− axis (in kg m2 ).
[Iy] moment of inertia of body around the y− axis (in kg m ).
[Iz] moment of inertia of body around the z− axis (in kg m2).
[cogx ] x− coordinate of center of gravity (COG ) of rigid body (in m )
with respect to the computational grid.
[cogy ] y− coordinate of center of gravity (COG ) of rigid body (in m ).
with respect to the computational grid.
[cogz ] z− coordinate of center of gravity (COG ) of rigid body (in m ).
with respect to the computational grid.
DOF this option indicates which of the six degrees of freedom of movement
of rigid bodies are to be included.
SURGE translation in the x− axis.
SWAY translation in the y− axis.
HEAVE translation in the z− axis.
ROLL rotation around the x− axis.
PITCH rotation around the y− axis.
YAW rotation around the z− axis.
MLINE with this option the user can determine coefficients for mooring lines.
[K] spring coefficient (in N/m ).
[B] damping coefficient (in Ns/m ).
[apbx ] x− component of attachment point at bed relative to COG (in m ).
[apby ] y− component of attachment point at bed relative to COG (in m ).
[apbz ] z− component of attachment point at bed relative to COG (in m ).
[apfx ] x− component of attachment point at body relative to COG (in m ).
[apfy ] y− component of attachment point at body relative to COG (in m ).
[apfz ] z− component of attachment point at body relative to COG (in m ).
[elen ] equilibrium length (in m ).
PRETENSION this option indicates whether pretension of mooring lines is to be included.
FENDER with this option the user can determine coefficients for fenders.
[K] spring coefficient (in N/m ).
[apfx ] x− component of attachment point at body relative to COG (in m ).
[apfy ] y− component of attachment point at body relative to COG (in m ).
[apfz ] z− component of attachment point at body relative to COG (in m ).](swashuse71x.svg)
![CONSTANT this option indicates that a dimensionless friction coefficient will be adopted.
[cf] dimensionless coefficient.
Default: [cf] = 0.002
Note that [cf ] is allowed to vary over the computational region; in that
case use the commands INPGRID FRICTION and READINP FRICTION to
define and read the friction data. The command FRICTION is still required
to define the type of friction expression. The value of [cf ] in this command
is then not required (it will be ignored ).
CHEZY indicates that the Chezy formula will be activated.
1∕2
[cf] Chezy coefficient (in m /s).
Default: [cf] = 65.
Note that [cf ] is allowed to vary over the computational region; in that
case use the commands INPGRID FRICTION and READINP FRICTION to
define and read the friction data. The command FRICTION is still required
to define the type of friction expression. The value of [cf ] in this command
is then not required (it will be ignored ).
MANNING indicates that the Manning formula will be activated.
[cf] Manning coe fficient (in m −1∕3 s).
Default: [cf] = 0.019
Note that [cf ] is allowed to vary over the computational region; in that
case use the commands INPGRID FRICTION and READINP FRICTION to
define and read the friction data. The command FRICTION is still required
to define the type of friction expression. The value of [cf ] in this command
is then not required (it will be ignored ).
COLEBROOK indicates that the Colebrook -White formula will be activated.
[h] Nikuradse roughness height (in m ).
Note that [h ] is allowed to vary over the computational region; in that case
use the commands INPGRID FRICTION and READINP FRICTION to define
and read the roughness heights. The command FRICTION is still required to
define the type of friction expression. The value of [h ] in this command is
then not required (it will be ignored).
LOGLAW indicates that the logarithmic wall law will be activated.
SMOOTH indicates that the bottom is smooth, i.e. the roughness height is zero.
This option can be used in the depth-averaged mode (a logarithmic velocity
profile is then assumed ). Note that this option must be combined with the
standard k − 𝜀 model in the multi-layered mode (see command VISC).
This option is default.
ROUGHNESS indicates that the bottom is rough and is determined by the roughness height.
This option can be used in the depth-averaged mode (a logarithmic velocity
profile is then assumed ). Note that this option must be combined with the
standard k − 𝜀 model in the multi-layered mode (see command VISC).
[h] Nikuradse roughness height (in m ).
Note that [h ] is allowed to vary over the computational region; in that case
use the commands INPGRID FRICTION and READINP FRICTION to define
and read the roughness heights. The command FRICTION is still required to
define the type of friction expression. The value of [h ] in this command is
then not required (it will be ignored).](swashuse87x.svg)
![HORIZONTAL indicates that the horizontal mixing will be activated.
CONSTANT this option indicates that a constant horizontal eddy viscosity will
be adopted.
[visc ] constant viscosity value (in m2/s ).
SMAGORIN indicates that the Smagorinsky model will be employed.
[cs] Smagorinsky constant.
Default: [cs] = 0.2
MIXING indicates that the Prandtl mixing length hypothesis will be used.
[lm] mixing length (in meters).
VERTICAL indicates that the vertical mixing will be activated.
KEPS indicates that the standard k − 𝜀 model will be used.
[cfk ] vegetative drag-related constant for turbulent kinetic energy.
Default: [cfk ] = 0.07
Note that this constant is only relevant when vegetation is
included (see command VEGETATION ).
ONLY MEANT FOR STRUCTURED GRIDS.
[cfe ] vegetative drag-related constant for dissipation rate.
Default: [cfe ] = 0.16
Note that this constant is only relevant when vegetation is
included (see command VEGETATION ).
ONLY MEANT FOR STRUCTURED GRIDS.
FULL indicates that the full three-dimensional turbulence modelling
will be activated.
Note that this option is in lieu of the above mixing options.
ONLY MEANT FOR STRUCTURED GRIDS.
KEPS indicates that the standard k − 𝜀 model will be used.
LINEAR indicates that the linear stress- strain relation will be employed.
This amounts to the application of the Boussinesq hypothesis
and is the default.
NONLINEAR indicates that the nonlinear stress-strain relationship of
Speziale (1987) will be used.](swashuse90x.svg)
![[size ] characteristic grain size of porous structure(s) (in m ).
Note that [size ] is allowed to vary over the computational region; in that
case use the commands INPGRID PSIZE and READINP PSIZE to define and
read the grain sizes of different porous structures. The value of [size ] in
this command is then not required (it will be ignored).
[height ] structure height (relative to the bottom in meters ). Both submerged and
emerged porous structures can be defined in this way. An emerged structure
is the default.
Default: [height ] = 99999.
Note that [height ] is allowed to vary over the computational region; in that
case use the commands INPGRID HSTRUC and READINP HSTRUC to define and
read the structure heights of different structures. The value of [height ] in
this command is then not required (it will be ignored).
[alpha0 ] dimensionless constant for laminar friction loss (surface friction).
Default: [alpha0 ] = 200.
[beta0 ] dimensionless constant for turbulent friction loss (form drag).
Default: [beta0 ] = 1.1
[wper ] characteristic wave period (either mean of peak period in s).
In case of wave interaction with porous structures this parameter is required.](swashuse93x.svg)
![[height ] the plant height per vertical segment (in m ).
[diamtr ] the diameter of each plant stand per vertical segment (in m ).
[nstems ] the number of plant stands per square meter for each segment.
Note that [nstems ] is allowed to vary over the computational region to
account for the zonation of vegetation. In that case use the commands
INPGRID NPLANTS and READINP NPLANTS to define and read the vegetation
density. The (vertically varying) value of [nstems ] in this command will
be multiplied with this horizontally varying plant density.
Default: [nstems ] = 1
[drag ] the drag coefficient per vertical segment.
INERTIA indicates that the inertia force will be included.
[cm] the added mass coefficient.
POROSITY indicates that the porosity effect will be included.
VERTICAL indicates that the drag force in vertical direction will be included.](swashuse96x.svg)
![2
[diff ] constant horizontal eddy diffusivity (in m /s).
[retur ] return time, the unit is indicated in the next option:
SEC unit seconds
MIN unit minutes
HR unit hours
DAY unit days
NONCOHES indicates that noncohesive suspended load transport (sand) will be
activated.
This is the default.
[size ] median sediment diameter (in μm ).
Note that if [size ] is not specified, no sedimentation and erosion will
be taken place at the bed.
COHESIVE indicates that cohesive suspended load transport (mud ) will be activated.
[tauce ] critical bed shear stress for erosion (in N/m2 ).
2
[taucd ] critical bed shear stress for deposition2(in N/m ).
[erate ] entrainment rate for erosion (in kg/m /s).
[fall ] fall velocity (in mm/s ).
In case of cohesive sediment transport this parameter is required.
For sand transport, [fall ] may not be given by the user, which
it will then be calculated based on the sediment diameter.
[snum ] Schmidt number for sediment.
Default: [snum ] = 0.7
[ak] empirical constant to reduce the Von Karman constant and thereby
the bed shear stress in sediment-laden bottom boundary layer.
Adams and Weatherly (1981) suggest [ak] = 5.5.
DENSITY this option indicates whether to include the density effect of
suspended sediment in the fluid mixture or not.
YES indicates that the mixture density will be computed.
This is the default.
NO indicates that the density of water will not be changed by the
presence of sediment in the water column.
ANTICREEP this option indicates whether to include the anti- creepage terms or not.
NOT FOR UNSTRUCTURED--------GRIDS.--
NONE indicates that the anti-creepage terms will not be included.
This is the default.
STANDARD indicates that the anti-creepage terms as derived from the local
transformation will be employed.
SVK indicates that the Stelling and Van Kester method will be adopted.](swashuse104x.svg)
![[alpha ] threshold parameter at which to initiate wave breaking.
Note: [alpha ] > 0.
Default: [alpha ] = 0.6
[beta ] threshold parameter at which to stop wave breaking.
Note: 0 < [beta] < [alpha ].
Default: [beta ] = 0.3](swashuse110x.svg)
![STANDARD this option indicates that the classical central differencing for the
vertical pressure gradient will be employed.
BOX this option indicates that the Keller-box scheme will be adopted.
This is the default.
[theta ] parameter for the 𝜃− method. [theta ] = 0.5 corresponds to the
Crank -Nicolson scheme and [theta ] = 1 to the implicit Euler
scheme.
Default: [theta ] = 1.0
SUBGRID this option indicates that the subgrid approach will be adopted.
Note: this option cannot be applied in the case of pressurized flow.
ONLY MEANT FOR STRUCTURED GRIDS.
[pmax ] number of vertical pressure layers and 1 ≤ [pmax ] ≤ kmax.
Default: [pmax ] = kmax
REDUCED this option indicates that the reduced pressure equation method will
be adopted.
Note: this option cannot be applied in the case of pressurized flow.
[qlay ] number of layers, started from the bottom layer, for which pressure is
constant in the vertical to reduce the pressure equation.
Default: [qlay ] = 1
SOLVER with this option the user can influence some of the numerical parameters
of iterative solvers.
[rhsaccur ] relative accuracy with respect to the right-hand side.
Default: [rhsaccur ] = 0.01
[initaccur ] relative accuracy with respect to the initial residual.
Default: [initaccur ] = 0.0
[maxiter ] maximum number of iterations.
Default: [maxiter ] = 500
[relax ] parameter for a linear solver:
∙ relaxation parameter for the ILU (D ) preconditioning. [relax ] = 0
corresponds to ILU (D) and [relax ] = 1 corresponds to MILU (D).
Default: model dependent (see above).
∙ under relaxation parameter for the SIP solver.
Default: [relax ] = 0.91
PRECONDI with this option the user can choose a preconditioner.
ONLY MEANT FOR STRUCTURED GRIDS.
ILUD indicates the ILUD preconditioner.
This is the default.
ILU indicates the ILU preconditioner.
PROJECTION with this option the user can choose the first order pressure projection
method instead of the default second order pressure correction method.
ITERATIVE with this option the accuracy of the pressure projection method is
improved through an iteration process.
[tol ] error tolerance to terminate the iteration process.
Default: [tol ] = 0.0001
[maxiter ] maximum number of iterations.
Default: [maxiter ] = 50](swashuse116x.svg)
| | UMOM MOMentum|HEAD / -> Horizontal |
| | \ Vertical |
| UPWind < |
| | WMOM / -> Horizontal |
| | \ Vertical |
| |
| CORRdep |
DISCRETization < > &
| TRANSPort / -> Horizontal |
| \ Vertical |
| |
| | -> Umom |
| ACURrent < |
| | Wmom |
| NONe |
| |
| FIRstorder |
| |
| HIGherorder [kappa] |
| |
| | -> SWEBy [phi] |
| | |
| LIMiter < RKAPpa [kappa] |
| | |
| | PLKAPpa [kappa] [mbound] |
| FROmm |
| |
| -> BDF|LUDs |
| |
< QUIck >
| |
| CUI |
| |
| MINMod |
| |
| SUPerbee |
| |
| VANLeer |
| |
| MUScl |
| |
| KORen |
| |
| SMArt |
With this optional command the user can influence the spatial discretization.
For advection-dominated flows it is possible that wiggles in the solution arise. In that case upwind discretization might be the appropriate choice. Three types of upwind schemes are implemented:
TVD schemes with several classes of flux limiters:
Schemes of up to third order accuracy can be constructed by piecewise polynomial interpolation, the
so-called κ−formulation. For all values of κ ∈ [−1, 1], a blended form arises between second order
backward difference scheme (BDF) and second order central differencing. The schemes BDF,
QUICK and CUI are obtained by setting κ = −1, 1/2 and 1/3, respectively. The value κ = 0
gives the Fromm’s scheme, while κ = 1 corresponds to central differencing. For κ≠1/3 the local
truncation error is of second order; for κ =1/3 it is of third order. By employing structured grids,
all upwind schemes are applied in each computational direction. Hence no streamline upwinding
is used.
Implementation of high resolution and TVD schemes on unstructured meshes is by far
non-trivial. Especially, the so-called r−ratio (measuring the local monotonicity and an argument
for the flux limiter) as it should comply the principles of the TVD theory. In UnSWASH, the
r−ratio formulation of Casulli and Zanolli (2005) is employed.
In case of transport equations for salinity, temperature, or suspended sediment (keyword
TRANSPORT) a TVD scheme must be applied to prevent wiggles in the solution or to avoid
negative concentration values.
The water depth in velocity points is not uniquely defined. An appropriate approximation is
based on first order upwinding instead of the usual interpolation. To achieve second order
accuracy in space, we add a higher order interpolation augmented with a flux limiter. See
keyword CORRDEP.
Conservation properties become crucial for rapidly varied flows. These properties are often
sufficient to get solutions that are acceptable in terms of local energy losses, location of incipient
wave breaking, propagation speed of a bore, etc. In flow expansions, the horizontal advective
terms in u− and v−momentum equations are approximated such that they are consistent with
momentum conservation; see option MOMENTUM. In flow contractions, the approximation is such
that constant energy head is preserved along a streamline, i.e. the Bernoulli equation; see option
HEAD.
With respect to unstructured triangular meshes, a robust and efficient upwind-biased scheme for
the horizontal advection terms in the momentum equation has been implemented [5]. The scheme
complies with the Rankine-Hugoniot jump relations and is specifically designed with a view to
preserving the local momentum flux. This is crucial to the simulation of breaking waves and
unsteady bores.
The default option is the second order backward difference (BDF) scheme (κ = −1) for all horizontal advective terms in both u∕v−momentum and w−momentum equations, and the MUSCL scheme for the vertical term in the u∕v−momentum equation and also in the w−momentum equation. The exception is when the BREAK command is employed, which in that case the central differences (κ = 1) are applied to all horizontal advective terms in the u∕v−momentum equations.
In addition, the water depth in velocity points is approximated with the MUSCL limiter. All the advection terms in any transport equation are approximated with the second order Van Leer limiter.
By default, SWASH decides whether energy head or momentum conservation is to be applied, though restricted to structured meshes. In principle, energy head conservation will be applied only in strong flow contractions, while elsewhere the momentum conservation is applied.
| MIN | | -> MEAN BOTCel < | MAX | | SHIFt
CANNOT BE USED IN CASE OF UNSTRUCTURED GRIDS.
With this optional command the user can determine how the bottom levels need to be computed
in cell centers.
The bottom levels are usually defined in the corners of computational cells. These
bottom levels have been extracted from the input grid (see command INPGRID BOTTOM).
Nevertheless, SWASH uses a staggered grid and to determine the total water depth at water
level points, a bottom level in the cell center is then required. As a rule, we take the
average bottom level from the surrounding bottom corners to determine the total depth
at cell center. This is fine for many cases. However, in the vicinity of steep bottom
slopes, use of the average bottom level may lead to an inaccurate flooding and drying
process (e.g. too much or too less volume of water left on tidal flats or flood plains) or
inaccurate tide propagation. Another example is the inaccurate computation of pressure in
front of the vertical wall which may negatively affect wave overtopping. For those
situations it is more appropriate to take the bottom level at cell center being equal to
the minimum of the surrounding bottom levels at the corner points. This so-called
tiled bottom approach is also suitable to represent a small channel of one grid cell
width.
Alternatively, it is possible to specify the bottom level at cell center as the maximum of the
surrounding bottom levels or being shifted from the upper-right corner of the computational cell.
This latter implies that, if the bottom input grid is identical to the computational grid in terms
of resolution and orientation, the user-defined bottom values are specified on input at cell centers
(instead of upper-right corners).
Note that for determining the bottom level in cell centers the positive downwards orientation is
considered. So the minimum operation results into the shallowest bottom level. As a
consequence, when the bottom level is above the reference level, i.e. a negative value, the
maximum operation should be chosen, instead of the minimum one, in the context of the tiled
bottom approach.
The default option is MEAN.
| EXPL [cfllow] [cflhig] | TIMEI METH < > & | IMPL [thetac] [thetas] SOLVer [tol] [maxiter] [weight] NEWTon | VERTical [thetau] [thetaw] [thetat]
With this optional command the user can influence the time integration.
Note that the default option depends on the choice of the computational mesh, either structured
or unstructured (see below).
If time integration is explicit, a time step restriction must be applied based on a Courant number
associated with the long wave speed. For definition, see Appendix A. Note that a maximum
Courant number of 0.5 is advised in case of high waves, nonlinearities (e.g. wave breaking,
wave-wave interactions), and wave interaction with structures with steep slopes (e.g. quays,
piers).
An automatic time step control is implemented as follows. The actual maximum of the Courant
number over all wet grid points is determined. The time step is halved when this number
becomes larger than a preset constant [cflhig] < 1, and the time step is doubled when this
number is smaller than another constant [cfllow], which is small enough to be sure the time
step can be doubled. Information on the actual time step changes is provided in the PRINT
file.
If time integration is semi-implicit, then the gradient of the water level in the momentum
equations and the velocity divergence in the (global) continuity equation are discretized
implicitly by means of the 𝜃−method, while both the horizontal advective and viscosity terms
are discretized explicitly. As a consequence, the stability of the method will not depend upon
the long wave speed. However, the time step will be restricted owing to the explicit
treatment of the horizontal advective terms, although this restriction is mild. This method
is particular useful and efficient for the simulation of three-dimensional circulation
driven by buoyancy, tides and winds, combined with unstructured meshes, as the wave
Courant number can easily be larger than 1 while still providing sufficiently accurate
solution.
This semi-implicit time stepping requires the solution of a system of linear equations to obtain
the water levels. This system is symmetric and positive definite and can be solved efficiently by
using a preconditioned conjugate gradient (PCG) method. The keyword SOLVER controls the use
of this iterative method. The iteration process stops if the norm of the residual falls below a
small fraction of the initial residual; this small fraction is the user prescribed error tolerance
[tol]. The preconditioner is a weighted combination of ILUD and its modified variant
MILUD in the case of structured grids and a weighted combination of ILU and MILU in
the case of triangular meshes. For details on the weighting parameter α, which may
improve the convergence, see command NONHYDROSTATIC. This parameter is indicated by
[weight].
Regarding the wet areas falling dry, the flow Courant number is required to be smaller or equal 1
[2]. Consult Section 5.4.6 for further details. Hence, this poses no additional restriction on the
time step in the case of explicit time integration. In contrast, there is a risk that the
water depth will become negative when semi-implicit time integration is applied as a
larger time step is allowed. As an alternative, one can instead enforce the depth to
be non-negative during the whole simulation. This introduces a nonlinear volume
term in the system of equations for the water levels that can be efficiently solved by a
Newton-type iteration method (Casulli, 2009). This can be activated with command
NEWTON.
When dealing with floating objects interacting with waves (e.g. a moored ship, WECs), the flow
is locally pressurized. In this case explicit methods cannot be employed. Instead, the
semi-implicit approach must be applied which amounts to the solution of a piecewise linear
system of equations to obtain the water levels for free surface flow and the piezometric
head for pressurized flow. Since each grid cell is labeled with either free surface or
pressurized in a proper way, this system can still be solved efficiently by the PCG solver.
Alternatively, the system of equations can also be solved by a nested Newton iteration
method as described in Brugnano and Casulli (2009), which may allow a larger time
step.
In the multi-layered mode, the vertical advective and viscosity terms in the momentum and transport equations are discretized implicitly by means of the 𝜃−method.
![METHOD with this option the type of time integration is indicated.
EXPLICIT indicates that the time integration is explicit.
This is the default for structured grids.
[cfllow ] minimum Courant number to be used for automatic time step control.
Default: [cfllow ] = 0.4
[cflhig ] maximum Courant number to be used for automatic time step control.
Default: [cflhig ] = 0.8
IMPLICIT indicates that the time integration is semi-implicit.
This is the default for unstructured meshes.
[thetac ] parameter for the 𝜃− method applied to the continuity equation.
[thetac ] = 0.5 corresponds to the Crank -Nicolson scheme and
[thetac ] = 1 to the implicit Euler scheme.
Default: [thetac ] = 0.5
[thetas ] parameter for the 𝜃− method applied to the water level gradient.
[thetas ] = 0.5 corresponds to the Crank -Nicolson scheme and
[thetas ] = 1 to the implicit Euler scheme.
Default: [thetas ] = 0.5
SOLVER with this option the user can influence some of the parameters of
the preconditioned conjugate gradient method.
[tol ] error tolerance to terminate the iteration process.
Default: [tol ] = 0.01
Note: in case of Newton iteration, the default is [tol ] = 0.001
[maxiter ] maximum number of iterations.
Default: [maxiter ] = 100
[weight ] weighting parameter for the (M )ILU (D) preconditioning.
[weight ] = 0 corresponds to ILU (D) and [weight ] = 1 corresponds
to MILU (D).
Default: [weight ] = 0.9
Note: in case of an unstructured mesh, the default is [weight ] = 0.
NEWTON indicates that the (nested) Newton iteration method is employed.
This is the default for unstructured meshes.
VERTICAL with this option the time integration of vertical terms is indicated.
[thetau ] parameter for the 𝜃− method in case of the u∕v− momentum equation.
[thetau ] = 0.5 corresponds to the Crank -Nicolson scheme and
[thetau ] = 1 to the implicit Euler scheme.
Default: [thetau ] = 0.5
[thetaw ] parameter for the 𝜃− method in case of the w− momentum equation.
[thetaw ] = 0.5 corresponds to the Crank -Nicolson scheme and
[thetaw ] = 1 to the implicit Euler scheme.
Default: [thetaw ] = 0.5
[thetat ] parameter for the 𝜃− method in case of the transport equation.
[thetat ] = 0.5 corresponds to the Crank -Nicolson scheme and
[thetat ] = 1 to the implicit Euler scheme.
Default: [thetat ] = 0.5](swashuse125x.svg)
There are two categories of output commands:
Locations
commands defining sets of output locations at which the user requires output. Each
set is indicated with a name (’sname’ in this manual) which must be unique and not
more than 8 characters long.
Types of sets of output points:
Commands RAY and ISOLINE cannot be used in 1D-MODE. If one gives one name for two sets of output locations, the first set is lost (first in the sequence in the command file). Three special names BOTTGRID, COMPGRID and NOGRID are reserved for use by SWASH (see below). The user may not define sets with these names.
Write / plot
commands defining data file output (write) at the above defined set(s) of output
locations:
Command BLOCK cannot be used in 1D-MODE.
FRAme ’sname’ [xpfr] [ypfr] [alpfr] [xlenfr] [ylenfr] [mxfr] [myfr])
With this optional command the user defines output on a rectangular, uniform grid in a regular
frame.
If the set of output locations is identical to a part of the computational grid, then the user can use the alternative command GROUP.
![’sname ’ name of the frame defined by this command
[xpfr ] x− coordinate of the origin of the frame in problem coordinates
--------------------
if Cartesian coordinates are used in m
if spherical coordinates are used in degrees (see command COORD )
[ypfr ] y− coordinate of the origin of the frame in problem-coordinates
if Cartesian coordinates are used in m
if spherical coordinates are used in degrees (see command COORD )
[alpfr ] direction of the x− axis of the frame (in degrees, Cartesian convention; must be
0 in case of spherical coordinates)
[xlenfr ] length of the frame in x− direction
if Cartesian coordinates are used in m
if spherical coordinates are used in degrees (see command COORD )
[ylenfr ] length of the frame in y− direction
if Cartesian coordinates are used in m
if spherical coordinates are used in degrees (see command COORD )
[mxfr ] number of meshes in x− direction of the rectangular grid in the frame (one less
than the number of grid points in this direction )
Default: [mxfr ]=20
[myfr ] number of meshes in y− direction of the rectangular grid in the frame (one less
than the number of grid points in this direction )
Default: [myfr ]=20](swashuse130x.svg)
Some output may be required on a frame that is identical with the bottom input grid or with the
computational grid. These frames need not be defined by the user with this command
FRAME; the frames are always generated automatically by SWASH under the names
’sname’ = ’BOTTGRID’ (for the bottom grid) and ’sname’ = ’COMPGRID’ (for the
computational grid).
GROUP ’sname’ SUBGrid [ix1] [ix2] [iy1] [iy2]
CANNOT BE USED IN CASE OF UNSTRUCTURED GRIDS.
With this optional command the user defines a group of output locations on a rectangular or
curvilinear grid that is identical with (part of) the computational grid (rectilinear or curvilinear).
Also, the flow variables (surface elevation, velocity components and pressure) will be outputted
in their points of definition according to the Arakawa C-grid staggering. Such a group
may be convenient for the user to obtain output that is not affected by interpolation
errors.
Command CGRID should precede this command GROUP.
The subgrid contains those points (ix,iy) of the computational grid for which:
[ix1] ≤ ix ≤ [ix2] and [iy1] ≤ iy ≤ [iy2]
For convenience the size of the group, the corner coordinates and the angle with the problem
coordinate system are written to PRINT file. The origin of the computational grid is
(ix=1,iy=1)!
![’sname ’ name of the set of output locations defined by this command
[ix1 ] lowest grid index of subgrid in terms of computational grid in ix-direction
[iy1 ] lowest grid index of subgrid in terms of computational grid in iy-direction
[ix2 ] highest grid index of subgrid in terms of computational grid in ix-direction
[iy2 ] highest grid index of subgrid in terms of computational grid in iy-direction](swashuse133x.svg)
Limitations:
[ix1]≥1, [ix2]≤[mxc]+1, [iy1]≥1, [iy2]≤[myc]+1 ([mxc] and [myc] as defined in the
command CGRID).
CURve ’sname’ [xp1] [yp1] < [int] [xp] [yp] >
With this optional command the user defines output along a curved line. Actually this curve is a broken line, defined by the user with its corner points. The values of the output quantities along the curve are interpolated from the computational grid. This command may be used more than once to define more curves.
RAY ’rname’ [xp1] [yp1] [xq1] [yq1] < [int] [xp] [yp] [xq] [yq] >
CANNOT BE USED IN 1D-MODE.
With this optional command the user provides SWASH with information to determine output
locations along the depth contour line(s) defined subsequently in command ISOLINE (see
below).
The locations are determined by SWASH as the intersections of the depth contour line(s) and the
set of straight rays defined in this command RAY. These rays are characterized by a set of master
rays defined by their start and end positions ([xp],[yp]) and ([xq],[yq]). Between each pair of
sequential master rays thus defined SWASH generates [int]−1 intermediate rays by linear
interpolation of the start and end positions.
Note that the rays thus defined have nothing in common with wave rays (e.g. as obtained from conventional refraction computations).
| -> DEPth | ISOline ’sname’ ’rname’ < > [dep] | BOTtom |
CANNOT BE USED IN 1D-MODE AND IN CASE OF CURVILINEAR GRIDS.
With this optional command the user defines a set of output locations along one depth or bottom level contour line (in combination with command RAY).
![’sname ’ name of the set of output locations defined by this command
’rname ’ name of the set of rays (as defined in command RAY )
DEPTH indicates the water depth, i.e. still water depth plus still water level
(see command SET) or still water depth plus initial spatially varying
water level (see command INPGRID WLEV ).
BOTTOM indicates the still water depth, i.e. the depth with respect to datum level.
[dep ] the depth (in meters) of the depth contour line along which output locations
are generated by SWASH.](swashuse142x.svg)
The set of output locations along the depth contour lines created with this command is of the
type CURVE.
| < [xp] [yp] > | POINts ’sname’ < > | FILE ’fname’ |
With this optional command the user defines a set of individual output locations (points). The coordinates of these points are given in the command itself or read from a file (option FILE).
![’sname ’ name of the points
[xp], [yp] problem coordinates of one output location
--------------------
if Cartesian coordinates are used in m
if spherical coordinates are used in degrees (see command COORD )
’fname ’ name of the file containing the output locations.](swashuse145x.svg)
| .......... | QUANTity < > ’short’ ’long’ [lexp] [hexp] [excv] & | .......... | [ref] (for output quantity TSEC) & [dur] SEC|MIN|HR|DAY (for output quantities SETUP, HSIG, HRMS, MVEL, MTKE and MSAL) & [depth] (for output quantity HRUN) & [delrp] (for output quantity RUNUP) & [xcom] [ycom] [zcom] (for output quantities MOMX, MOMY, MOMZ) & [alpobj] (for output quantities FORCEX, FORCEY, FORCEZ, MOMX, MOMY, MOMZ) & |-> PROBLEMcoord | < > (for directions and vectors, e.g. VDIR and VEL) | FRAME |
With this command the user can influence or specify
![|... |
< > the output parameters as given in commands BLOCK and TABLE.
|... |
‘short ’ user preferred short name of the output quantity (e.g. the name appearing in
the heading of a table written by SWASH ). If this option is not used, SWASH
will use a realistic name.
‘long ’ long name of the output quantity (e.g. the name appearing in the heading of a
block output written by SWASH ). If this option is not used, SWASH will use a
realistic name.
[lexp ] lowest expected value of the output quantity.
[hexp ] highest expected value of the output quantity; the highest expected value is
used by SWASH to determine the number of decimals in a table with heading.
So the QUANTITY command can be used in case the default number of decimals
in a table is unsatisfactory.
[excv ] in case there is no valid value (e.g. wave height in a dry point) this
exception value of the output quantity is written in a table or block output.](swashuse148x.svg)
The following data are accepted only in combination with some specific output quantities.
![[ref ] reference time used for the quantity TSEC.
Default value: starting time of the first computation, except in cases where
this is later than the time of the earliest input. In these cases, the time of
the earliest input is used.
[dur ] the time duration over which the wave parameters (e.g. wave height and
setup), mean current or mean turbulence quantities are computed. This
corresponds to the final stage of the simulation period, which should be
long enough to establish steady -state conditions. The corresponding unit
is indicated in the next option:
SEC unit seconds
MIN unit minutes
HR unit hours
DAY unit days
[depth ] the total depth (in m ) where inundation takes place. This can be used
to compute the maximum runup height; see output quantity HRUN.
[delrp ] the threshold depth (in m) for runup height calculation; see output
quantity RUNUP.
[xcom ] x− coordinate of center of mass of floating body (in m ) with respect to
the computational grid. To be used to compute the moments acting
on the body; see output quantities MOMX, MOMY and MOMZ.
Default: [xcom ] = 0.0
[ycom ] y− coordinate of center of mass of floating body (in m ).
Default: [ycom ] = 0.0
[zcom ] z− coordinate of center of mass of floating body (in m ).
Default: [zcom ] = 0.0
[alpobj ] direction of the positive x− axis of the floating object (in degrees, Cartesian
convention) with respect to the computational grid. To be used to compute
the forces and moments acting on the rotated body.
Default: [alpobj ] = 0.0
PROBLEMCOORD − vector components are relative to the x− and y− axes of the problem
coordinate system:
∙ directions are counterclockwise relative to the positive x− axis of the
problem coordinate system if Cartesian direction convention is used
--------
(see command SET )
∙ directions are relative to North (clockwise ) if Nautical direction
convention is used (see command SET )
FRAME If output is requested on sets created by command FRAME or automatically
(COMPGRID or BOTTGRID ):
∙ vector components are relative to the x− and y− axes of the frame--
coordinate system
∙ directions are counterclockwise relative to the positive x− axis of the
frame--coordinate system if Cartesian direction convention is used
(see command SET )
∙ directions are relative to North (clockwise ) if Nautical direction
convention is used (see command SET )](swashuse149x.svg)
Examples:
OUTPut OPTIons ’comment’ (TABle [field]) (BLOck [ndec] [len])
This command enables the user to influence the format of block and table output.
![UPWIND indicates the type of discretization for momentum equations.
UMOM indicates the discretization employed for u ∕v− momentum equation.
MOMENTUM indicates that momentum must be conserved everywhere.
HEAD indicates that energy head must be conserved everywhere.
HORIZONTAL indicates the discretization of the horizontal advective terms.
VERTICAL indicates the discretization of the vertical advective terms.
WMOM indicates the discretization employed for w − momentum equation.
CORRDEP indicates the type of discretization for water depth in velocity points.
TRANSPORT indicates the discretization employed for transport equation (s).
ACURRENT indicates the discretization of the advection terms added to the
momentum equations due to the ambient current.
NONE indicates that no upwinding is applied, hence the standard
central difference scheme is used.
This is the default in case of vertical advective terms.
FIRSTORDER indicates that the standard first order upwind scheme is used.
HIGHERORDE a higher order upwind κ − scheme is activated.
[kappa ] parameter defining the type of κ− scheme used.
For instance, [kappa ] = 0.5 gives the QUICK scheme
and [kappa ] = 0 the Fromm ’s scheme.
Note: − 1 ≤ [kappa ] ≤ 1.
LIMITER indicates that a TVD scheme with flux limiter must be applied.
SWEBY a Sweby limiter is activated.
[phi ] parameter defining the type of Sweby limiter used. For instance,
[phi ] = 1 defines the minmod limiter.
Note: 1 ≤ [phi] ≤ 2.
RKAPPA an R − κ limiter is activated.
PLKAPPA a PL − κ limiter is activated.
[mbound ] parameter indicating the upper bound of the PL − κ limiter.
Note: [mbound ] > 0.
FROMM indicates the Fromm ’s scheme.
BDF indicates the second order backward upwind scheme.
This is the default in case of horizontal advective terms.
QUICK indicates the QUICK scheme.
CUI indicates the CUI scheme.
MINMOD indicates the minmod limiter.
SUPERBEE indicates the superbee limiter.
VANLEER indicates the Van Leer limiter.
MUSCL indicates the MUSCL limiter.
This is the default in case of CORRDEP.
KOREN indicates the Koren limiter.
SMART indicates the SMART limiter.](swashuse119x.svg)
![’sname ’ name of the curve
[xp1 ],[yp1 ] problem coordinates of the first point of the curve
if Cartesian-coordinates are used in m
if spherical coordinates are used in degrees (see command COORD )
[int ] SWASH will generate output at [int ]− 1 equidistant locations between two
subsequent corner points of the curve
[xp], [yp] problem coordinates of a corner point of the curve. Repeat the group
[int ] [xp ] [yp ] in proper order if there are more corner points on the curve.](swashuse136x.svg)
![’rname ’ name of the set of rays defined by this command.
[xp1 ],[yp1 ],problem coordinates of the begin and end points of the first master ray
[xq1 ],[yq1 ] if Cartesian-coordinates are used in m
if spherical coordinates are used in degrees (see command COORD )
[int ] number of subdivisions between the previous master ray and the
following master ray defined by the following data (number of
subdivisions is one more than the number of interpolated rays)
[xp], [yp], problem coordinates of the begin and end points of each subsequent master ray
--------------------
[xq], [yq] if Cartesian coordinates are used in m
if spherical coordinates are used in degrees (see command COORD )](swashuse139x.svg)
| -> HEADer |
BLOck ’sname’ < > ’fname’ (LAYout [idla])
| NOHEADer |
| DEP |
| |
| BOTL |
| |
| WATL |
| |
| DRAF |
| |
| VMAG |
| |
| VDIR |
| |
| VEL |
| |
| VKSI |
| |
| VETA |
| |
| PRESS |
| |
| NHPRES |
| |
| QMAG |
| |
| QDIR |
| |
| DISCH |
| |
| QKSI |
| |
| QETA |
| |
| VORT |
| |
| WMAG |
| |
| WDIR |
| |
| WIND |
| |
| FRC |
| |
| USTAR |
| |
| UFRIC |
| |
| SAL |
| |
| TEMP |
| |
| SED |
| |
| HRUN |
| |
| BRKP |
| |
| SETUP |
| |
| HS |
| |
| HRMS |
| |
| MVMAG |
| |
| MVDIR |
| |
| MVEL |
| |
| MVKSI |
| |
| MVETA |
| |
| MSAL |
| |
| MTEMP |
| |
| MSED |
| |
| ZK |
| |
| HK |
| |
| VMAGK |
| |
| VDIRK |
| |
| VELK |
| |
| VKSIK |
| | | -> Sec |
< < VETAK > [unit] > (OUTput [tbegblk] [deltblk]) < MIn >)
| | | HR |
| VZ | | DAy |
| |
| VOMEGA |
| |
| SALK |
| |
| TEMPK |
| |
| SEDK |
| |
| TKE |
| |
| EPS |
| |
| VISC |
| |
| QMAGK |
| |
| QDIRK |
| |
| DISCHK |
| |
| QKSIK |
| |
| QETAK |
| |
| PRESSK |
| |
| NHPRSK |
| |
| MVMAGK |
| |
| MVDIRK |
| |
| MVELK |
| |
| MVKSIK |
| |
| MVETAK |
| |
| MSALK |
| |
| MTEMPK |
| |
| MSEDK |
| |
| MTKE |
| |
| MEPS |
| |
| MVISC |
| |
| TIME |
| |
| TSEC |
| |
| XP |
| |
| YP |
| |
| DIST |
| |
| FORCEX |
| |
| FORCEY |
| |
| FORCEZ |
| |
| MOMX |
| |
| MOMY |
| |
| MOMZ |
| |
| TRAX |
| |
| TRAY |
| |
| TRAZ |
| |
| ROTX |
| |
| ROTY |
| |
| ROTZ |
| |
| PTOP |
| |
| RUNUP |
With this optional command the user indicates that one or more spatial distributions should be written to a file.
![’sname ’ name of frame or group (see commands FRAME or GROUP )
HEADER with this option the user indicates that the output should be written to a file
with header lines. The text of the header indicates run identification (see
command PROJECT ), time, frame name or group name (’sname ’), variable and
unit. The number of header lines is 8.
Note: the numerical values in the file are in the units indicated in the header.
NOHEADER with this option the user indicates that the output should be written to a file
without header lines.
’fname ’ name of the data file where the output is to be written to.
Default for option HEADER is the PRINT file. In case of NOHEADER the
filename is required. Below a few remarks on the file formats.
Basically, the output files generated by SWASH are human -readable files that
use ASCII character encoding. Such files can be open and edit in any text editor
or can be viewed in Matlab or Excel. However, if the user specifies the extension
of the output file as ‘.mat ’, a binary MATLAB file will be generated. This file
requires less space on your computer and can be loaded in MATLAB much faster
than an ASCII file. Also note that the output parameters are stored as single
precision. (Hence, use the Matlab command double for conversion to double
precision, if necessary.) Binary MATLAB files are particularly useful for the
computation with unstructured grids. A number of MATLAB scripts are
provided with the SWASH source code that can be used to plot wave parameters
as maps in a simple way.
Since version 8.01, SWASH can generate VTK files that can be viewed in
Paraview, an open -source, general-purpose visualization package, available for
Windows, Mac and Linux (see https://www.paraview.org ). The basic extension
is ‘.vtk’, but SWASH will generate various XML -based file formats depending
on the grid types (*.vts associated with structured grids and *.vtu containing
unstructured mesh data). The VTK XML files are binary, self-descriptive
(include plain text metadata ) and portable (cross- platform ). In addition, a
key bene fit is that there is no need to collect VTK files residing on separate
processes of a distributed memory machine (after execution of SWASH in
parallel). Paraview can simply visualize the whole domain that consists of
several subdomains.
LAY- OUT with this option the user can prescribe the lay-out of the output to file with
the value of [idla ].
[idla ] see command READINP (options are: [idla ]=1, 3, 4). Option 4 is recommended
for postprocessing by MATLAB, however, in case of a generated binary
MATLAB file option 3 is recommended.
Default: [idla ] = 1
DEPTH water depth (in m ) (not the still water depth!).
BOTLEV bottom level or still water depth (in m ).
Output is in both active and non -active points.
Note: exception value for bottom levels must be given!
(See command INPGRID BOTTOM EXCEPTION ).
WATLEV water level or surface elevation (in m ).
Output is in both active and non -active points.
Note: exception value for water levels must be given!
(See command INPGRID WLEVEL EXCEPTION ).
DRAFT draft of floating object (in m ).
Output is in both active and non -active points.
VMAG velocity magnitude (in m/s ).
VDIR velocity direction (in degrees; Cartesian or nautical; see command SET ).
VEL flow velocity (vector; in m/s ).
VKSI grid-oriented U -velocity (in m/s ).
Note: not applicable to unstructured meshes.
VETA grid-oriented V -velocity (in m/s ).
Note: not applicable to unstructured meshes.
PRESS pressure at bottom (in hPa ).
NHPRES normalised (by density) non -hydrostatic pressure at bottom (in m2/s2 ).
2
QMAG magnitude of discharge per unit width (in m /s).
QDIR direction of discharge per unit width (in degrees; Cartesian or nautical).
DISCH discharge per unit width (vector; in m2/s).
QKSI grid-oriented U -discharge per unit width (in m2/s ).
Note: not applicable to unstructured meshes.
2
QETA grid-oriented V -discharge per unit width (in m /s).
Note: not applicable to unstructured meshes.
VORT vorticity or rotation of the fluid in depth -averaged flow (in 1/s).
WMAG wind velocity at 10 m above sea level (in m/s ).
WDIR wind direction at 10 m above sea level (in degrees; Cartesian or nautical).
WIND wind velocity at 10 m above sea level (vector; in m/s ).
FRC bottom friction coefficient (see command FRICTION ).
USTAR magnitude of friction velocity (in m/s ).
UFRIC friction velocity (vector; in m/s ).
SAL salinity (in ppto).
TEMP temperature ( C).
SED suspended sediment (in kg/m3 ).
HRUN represents the maximum horizontal runup by masking inundated points
as 1 and non -inundated points as 0.
BRKP represents area of wave breaking by masking breaking points as 1
and non -breaking points as 0.
SETUP wave -induced setup (in m ).
HSIG significant wave height (in m; for definition, see Appendix A).
HRMS RMS wave height (in m; for definition, see Appendix A).
MVMAG time-averaged or mean velocity magnitude (in m/s ).
MVDIR time-averaged or mean velocity direction (in degrees; Cartesian or nautical;
see command SET).
MVEL time-averaged or mean velocity (vector; in m/s ).
MVKSI time-averaged or mean grid-oriented U -velocity (in m/s).
Note: not applicable to unstructured meshes.
MVETA time-averaged or mean grid-oriented V -velocity (in m/s).
Note: not applicable to unstructured meshes.
MSAL time-averaged or mean salinity (in ppt ).](swashuse156x.svg)
Notes:
For a proper use of the quantity HRUN, take into account the following notes:
To find and plot the location of inundation use the following Matlab script:
BWs=edge(Hrunup,’sobel’);
hrp=zeros(size(BWs,1),size(BWs,2));
hrp(BWs==1)=1;
hrp(hrp==0)=NaN;
x=Xp(find(hrp==1));
y=Yp(find(hrp==1));
Note the quantities XP and YP must be included as well.
The runup height RUNUP is computed by the intersection between free surface and bottom level. Three assumptions have been made for the calculation of this runup height.
This output quantity is space independent, can be specified with the command TABLE only, and the empty set NOGRID must be chosen.
| -> HEADer | | | TABle ’sname’ < NOHEADer > ’fname’ & | | | SWASH | | ... | | -> Sec | < < > > (OUTput [tbegtbl] [delttbl] < MIn >) | ... | | HR | | DAy |
With this optional command the user indicates that for each location of the output location set
’sname’ (see commands POINTS, CURVE, FRAME or GROUP) one or more variables should be
written to a file. Some quantities are space independent and vary in time only. These are e.g. the
wave runup height and the hydrodynamic loads (forces and moments acting on a floating object).
For these quantities an empty output set with the name ’sname’ = ’NOGRID’ must be
chosen.
The keywords HEADER and NOHEADER determine the appearance of the table; the filename determines the destination of the data.
![’sname ’ name of the set of POINTS, CURVE, FRAME, GROUP or the empty set NOGRID.
HEADer output is written in fixed format to file with headers giving name of variable
and unit per column. A disadvantage of this option is that the data are written
in fixed format; numbers too large to be written will be shown as: ****.
Number of header lines is 4.
NOHEADer output is written in floating point format to file and has no headers; it is
intended primarily for processing by other programs. With some spreadsheet
programs, however, the HEADER option works better.
SWASH a table on file is produced with a special fixed format appropriate for
layer- dependent quantities. This file contains headers with useful
information for a correct interpretation of the data.
’fname ’ name of the data file where the output is to be written to.
Default for option HEADER is output to the PRINT file.
In case of NOHEADER the filename is required.
|... |
< > the output parameters as given in command BLOCK.
|... |
OUTPUT the user requests output at various times. If the user does not use this option,
the program will give TABLE output for the last time step of the computation.
[tbegtbl ] begin time of the first field of the variable, the format is:
1 : ISO -notation 19870530.153000
2 : (as in HP compiler ) ’30− May − 87 15:30:00’
3 : (as in Lahey compiler) 05/30/87.15:30:00
4 : 15:30:00
5 : 87/05/30 15:30:00’
6 : as in WAM 8705301530
7 : 153000.000
This format is installation dependent. See Implementation Manual or ask the
person who installed SWASH on your computer. Default is option 7.
[delttbl ] time interval between fields, the unit is indicated in the next option:
SEC unit seconds
MIN unit minutes
HR unit hours
DAY unit days](swashuse159x.svg)
Notes:
| | < [i] [j] > | | | -> IJ < > | TEST [itest] [itrace] POINTS < | < [k] > | > & | | | XY < [x] [y] > | (FILE ‘fname’)
If SWASH produces unexpected results, this optional command can be used to instruct the program to produce intermediate results during a SWASH run (test output). A TEST command may change between commands in the file to change the level of test output during a SWASH run. This change occurs during the execution of the run. A TEST command controls the test output until the next TEST command. Such a next TEST command may have level 0, thus stopping test output.
![[itest ] the level of test output. For values under 100 the amount is usually reasonable,
for values above 200 it can be very large. For values of [itest ] up to 50 the
test output can be interpreted by the user. For higher values of [itest ] the
test output can only be interpreted by those who have the program source
listing at their disposal.
For instance, with [itest ] = 30, one may check mass and energy conservation,
if appropriate.
Default: [itest ] = 1
[itrace ] SWASH writes a message (name of subroutine) to the PRINT file at the first
[itrace ] entries of each subroutine.
Default: [itrace ] = 0
POINTS if this option is used, the user instructs SWASH to produce detailed print output
during the computational process for a grid point of the computational grid.
Output at a maximum of 50 grid points is possible. This option can be used
only after the bathymetry has been read (see command READINP BOTTOM ).
IJ the test points are defined by means of grid indices.
[i], [j] grid indices of a test point. Values of [i] range from 1 to [mxc ]+1
(see command CGRID ), values of [j] from 1 to [myc ]+1.
ONLY MEANT FOR STRUCTURED GRIDS.
[k] vertex index of a test point. This can be obtained in a grid generator file
(.node and .n files of Triangle and Easymesh, respectively ).
ONLY MEANT FOR UNSTRUCTURED GRIDS.
XY the test points are defined in terms of problem coordinates; SWASH will determine
the nearest grid points. Output will be made for this selected grid point.
[x], [y] coordinates of a test point (problem coordinates in meters in case of Cartesian
coordinates, or longitude and latitude in degrees in case of spherical coordinates,
see command COORD ).
FILE some flow variables for test points are written.
‘fname ’ name of the file to which the output is written; default filename: DIAGNOSTIC.](swashuse162x.svg)
| -> Sec | COMPute [tbegc] [deltc] < MIn > [tendc] | HR | | DAy |
This command orders SWASH to start the computation.
![[tbegc ] the start (date and ) time of the computation, the format is
1 : ISO -notation 19870530.153000
2 : (as in HP compiler ) ’30− May − 87 15:30:00’
3 : (as in Lahey compiler) 05/30/87.15:30:00
4 : 15:30:00
5 : 87/05/30 15:30:00’
6 : as in WAM 8705301530
7 : 153000.000
This format is installation dependent. See Implementation Manual or ask the
person who installed SWASH on your computer. Default is option 7.
[deltc ] the time step of the computation, the unit is indicated in the
next option:
SEC unit seconds
MIN unit minutes
HR unit hours
DAY unit days
[tendc ] the end time of the computation, format see [tbegc ].](swashuse165x.svg)
Note that several commands COMPUTE can appear, where the wave state at the end of one computation is used as initial state for the next one, unless a command INIT appears in between the two COMPUTE commands. This enables the user to change the computational time step during the whole computation, to change a boundary condition, to modify numerical parameters etc.
STOP
This required command marks the end of the commands in the command file. Note that the command STOP may be the last command in the input file; any information in the input file beyond this command is ignored.
In this chapter some guidelines for setting up a command file is given. This file contains all the necessary commands and data required for defining a model and running the simulation. All the commands and keywords are listed in Appendix C. Not all the commands need to be specified. Most of them will be taken default. Generally, a command file consists of five parts which must be specified by the user:
A distinction is made between the definition of grids in horizontal and vertical directions. In the
horizontal direction, either rectilinear, curvilinear or unstructured mesh can be employed. The
grid definition in vertical direction is defined by means of a fixed number of layers in a such a
way that both the bottom topography and the free surface can be accurately represented; see
also Figure 5.1.
First we need to define the size and direction of the computational domain in the
horizontal plane. The area of interest should be kept at least two wave lengths away from
the boundaries. Note that if a sponge layer needs to be included, the computational
domain needs to be extended with the size of that sponge layer. It is always wise
to choose the grid axes being aligned as much as possible with the dominant wave
direction.
An important aspect of specifying a computational grid is the spatial resolution. In principle,
most energetic wave components need to be resolved accurately on the grid. Basically, we take
sufficient number of grid points per wave length associated with the peak wave energy. For low
waves, i.e. H∕d ≪ 1 with H a characteristic wave height (either significant or RMS) and d the
(still) water depth, it is sufficient to take 50 grid cells (or 51 grid points) per peak wave length.
However, for relatively high waves, it is better to take at least 100 grid cells per peak wave
length. So, at least, we need to know something about a typical water depth and a typical peak
period. Based on the linear dispersion relation the corresponding peak wave length can be
found.
An example. We have a domain of 1500 m alongshore and 1200 m cross-shore of which the
deepest part is 20 m. We impose a wave spectrum at the entrance with a significant wave height
of 2 m and a peak period of 10 s. According to the linear dispersion relation the peak wave
length is about 120 m and Hs∕d = 0.1. Hence, the waves are not too low but also not too high
either. So, for safety, we choose 100 grid cells per peak wave length which implies a grid size of
1.2 m. Since the dominant wave direction is cross-shore, we may relax the grid size alongshore by
choosing 3 m. So, the total number of grid cells for the computational domain would be 500 ×
1000.
Keep in mind, however, that waves become shorter when the water depth decreases. Hence, for a
desired number of grid cells per wave length the grid resolution must therefore be higher locally.
In this respect, a rectangular, non-uniform grid is recommended. The desired number of grid cells
for this case may be lesser than the one associated with the peak wave length. A rule of thumb is
15 to 20 cells.
However, to further enhance the flexibility with respect to local grid refinements at places where
needed, either a boundary-fitted, orthogonal curvilinear grid or an unstructured triangular mesh
may be applied. Such meshes must be generated externally. The user is, however, strongly
advised to define the computational domain as a rectangle with one of the axis being aligned
with the dominant wave direction.
Another issue is the choice of the number of layers. This choice mainly depends on two types of application:
since flows and waves have drastically different physical features. If one is interested in the vertical flow structures, e.g. undertow and stratified flows, then at least 10 or perhaps more vertical layers should be adopted. If necessary, a non-equidistant layer distribution can be specified; see Figure 5.1. The layer thickness hk, which is the distance between two consecutive layer interfaces, may be defined in a relative way, i.e. a percentage of the water depth similar to the σ−coordinates, or in an absolute way, i.e. a constant or fixed layer thickness as expressed in meters. To make sure that the sum of the layer thicknesses equals the water depth, at least one layer must be defined in a relative way.
The choice for fixed layers may be useful in the case of a bathymetry exhibiting strong
variation of the depth, such as a lake with some pits, in order to keep the vertical resolution
relatively high along the bottom.
Concerning the wave transformation, the number of layers is determined by the linear frequency
dispersion. In particular, the dimensionless depth, kd with k the wave number, decides the
number of layers. The higher the value of kd, the more vertical layers needed. In addition, the
accuracy with which the phase velocity of the wave components, c = ω∕k with ω the angular
frequency, is obtained depends on the discretization of the vertical pressure gradient in the
momentum equations. For wave transformation usually the Keller-box scheme is adopted; see
Section 5.4.3.
The range of applicability of the SWASH model to values of kd indicating the relative importance of linear wave dispersion for primary waves is given in Table 5.1. This range is determined by requiring
| K | range | error |
| 1 | kd ≤ 0.5 | 1% |
| 1 | kd ≤ 2.9 | 3% |
| 2 | kd ≤ 7.7 | 1% |
| 3 | kd ≤ 16.4 | 1% |
a relative error in the normalized wave celerity (= c∕
) of at most 1%. An exception is the
use of one vertical layer where the relative error is 3%, which is acceptable for many
applications. Here, at most three layers may be considered enough for typical wave
simulations. Moreover, the layers are assumed to have variable thicknesses and be
equally distributed, which is the usual choice for wave simulations. So, do not use fixed
layers!
It is noted that SWASH uses its own dispersion relation, which is an approximate one of the exact linear dispersion relation, given by
This approximate relation is derived using the Keller-box scheme (see Section 5.4.3) and depends on the number of equidistant layers employed in the model. The linear dispersion relation of SWASH using one vertical layer, i.e. depth-averaged, is given by
while for two and three equidistant layers, it is given by
and
respectively. Thus the approximate dispersion relation is consistent with the model, particularly
for relatively high wave frequencies. This will lead to more accurate results. The approximate
dispersion relation in SWASH is only available for one, two and three equidistant layers with
variable thickness (i.e. sigma planes, not fixed layers). SWASH shall indicate this in the PRINT
file.
So, for primary waves with kd ≤ 2.9, use of one layer is sufficient, while at least two equidistant
layers need to be chosen if kd ≤ 7.7. For most typical nearshore wave simulations, two
layers may be enough. In the example above, kd = 1.04, so one vertical layer would be
enough.
However, one must realized that, for a given number of layers, relatively high harmonics may propagate too slow at a given depth. For example, using one layer, SWASH is accurate up to a kd value of 2.9 for primary waves. For a depth of 20 m (deepest part in the example above), the shortest wave that can accurately modelled at this depth has a frequency of 0.18 Hz (minimum wave period of 5.6 s; derived from the approximate dispersion relation above). In other words, for a given number of layers and a water depth, there is a maximum frequency above which a wave component has an incorrect celerity; see Table 5.2. This means, for instance, that the phase differences between the concerning harmonics are wrong.
| d (m) | K=1 | K=2 | K=3 |
| 1 | 0.82 | 1.37 | 2.00 |
| 5 | 0.37 | 0.61 | 0.89 |
| 10 | 0.26 | 0.43 | 0.63 |
| 15 | 0.21 | 0.35 | 0.52 |
| 20 | 0.18 | 0.31 | 0.45 |
| 25 | 0.16 | 0.27 | 0.40 |
| 30 | 0.15 | 0.25 | 0.36 |
| 35 | 0.14 | 0.23 | 0.34 |
| 40 | 0.13 | 0.22 | 0.32 |
| 45 | 0.12 | 0.20 | 0.30 |
| 50 | 0.12 | 0.19 | 0.28 |
| 100 | 0.08 | 0.14 | 0.20 |
This is particularly important when nonlinear effects are
dominant1 .
Ideally, the maximum frequency is about 1.5 to 2 times the peak frequency at a given depth. It is
then assumed that all components above this maximum frequency have a little bit amount of
energy (here the presuming spectrum shape is a Jonswap one). As a consequence, the phase
differences between the representative wave components, including the relatively short waves, are
thus well controlled in the model.
Referred to the example above, the peak frequency at the wavemaker boundary is 0.1 Hz, while the depth is 20 m. The required maximum frequency should be at least 0.15 Hz or preferably higher. So, the use of one layer would be critical when propagation of short waves with frequencies higher than 0.18 Hz needs to be modelled accurately.
The most important input grid is the bathymetric grid. This grid represents the bottom level at
each grid point with land points defined as negative while wet points are defined as
positive. The resolution of bathymetric grid is not necessarily the same as that of the
computational grid. It is advised to avoid extremely steep bottom slopes or sharp
obstacles as much as possible. Some kind of smoothing or re-interpolation is therefore
recommended.
Jetties, piers and quays, or other impermeable walls, may be schematized either
From a stability point of view, the second option is the best one. However, the first option may be a
better choice when, for instance, wave diffraction around the berm of the quay need to be
simulated accurately. To avoid unrealistically high surface elevation around the quays or
possible instabilities due to steep slopes, this first option may be combine with a larger
threshold of the water depth; see Section 5.4.6 and command SET DEPMIN. The default
value of this threshold is 0.05 mm. Depending on the horizontal grid sizes (Δx, Δy),
and thereby the actual slope, this threshold may be altered in order to get a stable
solution. The larger the grid sizes, the higher this threshold should be set (e.g. 0.1 mm or
even 1 mm). But be careful as this higher threshold may negatively influence mass
conservation.
Instead, however, a combination is also possible, i.e. to place the porosity layer on top
of the quay walls, and having a volumetric porosity of 20% and a grain size of 0.1
m.
A rubble mound breakwater must be schematized by means of porosity layers. These layers must
be placed inside the computational domain. Rubble mound breakwaters have a typical porosity
value of (n=) 0.4, while the stone size of the armour layer is typically 0.5 m. The berm of the
breakwater can be specified by means of the structure heights (relative to the bottom). In case of
two or more breakwaters in the domain, both porosity and structure height are thus spatially
varied, and so they need to be inputted by means of input grids. Also stone diameters need to be
specified as well.
Alternatively, the porosity layers may be placed on top of the impermeable core of the
breakwater which, in turn, is schematized by adapting the bottom level. In addition, the berm of
the breakwater is schematized by including its slope in the adapted bathymetry.
The width of the breakwater should be at least four times the grid size of the computational
grid. So, the grid resolution should be high enough. When choosing a too coarse grid size,
it may lead to an overestimation of the transmission and an underestimation of the
reflection.
This way of schematization permits to simulate partial reflection and transmission of the waves
through breakwaters. Wave reflection at a breakwater is typically determined by wave energy
dissipation on the slope and wave penetration into the breakwater. Both processes are equally
important, and thus both slope angle and porosity are important governing parameters for the
wave reflection.
Using the command INPGRID BOTTOM EXCEPTION, one can introduce permanently dry
points in the computational grid. This provides a means to make a line of dams or
screens through the computational domain, separating the flow on both sides. This line
of thin dams may represent a small obstacle with subgrid dimensions that possibly
influence the local flow. It must be noted that for parallel runs using MPI the user must
indicate an exception value for bottom levels, if appropriate, in order to obtain good load
balancing.
The water depth should be uniform along the wavemaker boundary where incident waves are
imposed.
If tidal currents are significant over the computational domain, the spatial distribution of the currents u(x,y) should be specified as an input grid.
To solve the continuity and momentum equations, appropriate boundary conditions need to be
imposed at the boundaries of the computational grid.
In general, initial conditions are more important for relative short simulations (e.g. a few minutes
in case of short waves or a few days in case of tidal waves). Boundary conditions are by far more
important for longer simulations. Moreover, often no information is available in order to start the
simulation. Therefore, the simulation will usually start with zero velocities and a spatially
constant water level, and the simulation will be long enough to get a steady-state solution; see
also Section 5.4.1.
Waves may be generated along one or two boundaries. These are called wavemaker boundaries.
First, it is assumed that the boundaries are not curved. Thus, the use of curvilinear grids is
restricted to rectangular domains with non-uniform grids. Second, it is assumed that the
variation of the depth along these wavemaker boundaries is slowly or (preferably) constant.
Third, it is advised to place these wavemaker boundaries away from the area of interest, and
away from steep topography. At the wavemaker boundary, we may imposed either regular or
irregular waves. For one-dimensional cases they are by definition long-crested or uni-directional.
For a two-dimensional case short-crested or multi-directional waves can also be specified. Usually,
a time series need to be given for incident waves. This may either be synthesized from
parametric information (wave height, period, etc.) or derived from a surface elevation time
series.
It is important to note that at a wavemaker boundary only the horizontal velocities (u and v) are
prescribed whereas a homogeneous Neumann condition is applied to the vertical velocity w. This,
however, may induce an error in the generating waves near the boundary, especially when the
waves are high and the advection terms of the w−momentum equation are involved.
Therefore, it is advised not to include (both horizontal and vertical) advection terms in the
w−momentum equation. (The balance between the local acceleration term ∂w∕∂t and
the vertical pressure gradient ∂q∕∂z usually suffices.) See Section 5.4.5 for further
details.
For regular waves, at least the wave height and the wave period must be specified.
Optionally, the wave direction can be specified as well. Alternatively, a time series can be
imposed.
For irregular waves, either a spectrum or time series can be enforced. In the case of a spectrum,
both the shape and wave characteristics need to be specified. The usual shape is either Jonswap
or Pierson-Moskowitz. Sometimes a TMA shape is desired. The wave characteristics are
determined by the following parameters: the significant or RMS wave height, peak or first order
mean period, peak wave direction, and directional spreading (only in case of short-crested
waves). The frequency range [fmin,fmax] is such that the highest frequency, fmax, equals 3 times
the peak frequency (or mean frequency), while the lowest one, fmin, equals half of the
peak/mean frequency.
Alternatively, a spectrum file may be given. There are two types of files:
Using a spectrum a time series of surface elevation will be synthesized. At least, the length of this series should correspond to the time period over which surface elevation and velocities are outputted after steady-state condition has been established. This time period should be long enough to provide statistically reliable wave data. After this time period the time series repeats itself. This duration of the time series is called the cycle period (see command BOUnd ... SPECTrum ... [cycle]). The recommended range is from 100 to 300 wave periods. If the cycle period is denoted as Tcycle, then the frequency step Δf to be used for the evaluation of the parametric spectrum (e.g. Jonswap) equals
Thus the spectrum is divided into N frequency bins with uniform spacing Δf,
Referring to the above example, we impose a Jonswap spectrum at the wavemaker boundary.
The peak period is 10 s, so that the frequencies are in between 0.05 Hz and 0.3 Hz. The duration
of the time series of surface elevation to be synthesized is set to 30 minutes, which is supposed to
be accurate enough to get sufficient statistics like wave height and mean period. Hence, in
total, 450 wave components will be generated at the entrance of the computational
domain.
Please be careful in choosing the cycle period. The larger this period the more wave components
will be involved at the wavemaker boundary. Based on these components, SWASH will synthesize
time series for the orbital velocities in each grid point and each vertical layer along the boundary.
That would enhance the computing time significantly.
When imposing a spectrum at the boundary, one has to realize that some so-called evanescent modes might be included as well. These modes show exponential decay with distance from the boundary at which the spectrum is imposed. As such, they can not be ”seen” by the model. Evanescent waves are a general property of the underlying model equations. The frequency at which the evanescent modes are generated is the cut-off frequency and is determined by the dispersive properties of the model equations. It is given by
with K the number of layers used in the model. Hence, the lowest wave period to be considered in the model simulation equals 2π∕ωcf. So, given the depth at the boundary and the number of layers used, the cut-off frequency is determined above which the evanescent waves are generated at the wavemaker boundary where the spectrum is imposed; see Table 5.3.
| d (m) | K=1 | K=2 | K=3 |
| 1 | 1.00 | 1.99 | 2.99 |
| 5 | 0.45 | 0.89 | 1.34 |
| 10 | 0.32 | 0.63 | 0.95 |
| 15 | 0.26 | 0.51 | 0.77 |
| 20 | 0.22 | 0.45 | 0.67 |
| 25 | 0.20 | 0.40 | 0.60 |
| 30 | 0.18 | 0.36 | 0.55 |
| 35 | 0.17 | 0.34 | 0.51 |
| 40 | 0.16 | 0.32 | 0.47 |
| 45 | 0.15 | 0.30 | 0.45 |
| 50 | 0.14 | 0.28 | 0.42 |
| 100 | 0.10 | 0.20 | 0.30 |
These evanescent modes will be removed by SWASH. Note that these modes carry a little
bit energy and thus negligible. SWASH will give a warning when at least 10% of the
total wave components are the evanescent modes that have been removed. If there
are too much evanescent modes on the boundary, i.e. these modes together contain a
significant amount of energy of the wave spectrum, the user is advised either to enlarge the
number of layers (see also Table 5.2) or to truncate the imposed spectrum (e.g. SWAN
spectrum), i.e. the highest frequency of the spectrum is not larger than the given cut-off
frequency.
In the above example, one layer (K = 1) has been chosen. We assume that along the wavemaker
boundary we have a uniform depth of 20 m. So the cut-off frequency is 0.22 Hz (see Table 5.3;
the lowest wave period is thus 4.5 s). However, the highest frequency is 0.3 Hz. So there are 144
evanescent modes on the boundary, which is about 30%, thus reasonably. They will be removed
from the boundary.
For high waves, sub- and super-harmonics are generated due to nonlinearity. These waves are
called bound waves as they are attached to the primary wave and travel at its phase speed
instead of that of a free wave at the same frequency. If linear wave conditions are enforced at the
boundaries, the model will generate spurious free wave components with the same magnitude but
180o out of phase with the bound waves at the wavemaker in order to satisfy the linear wave
boundary condition. The presence of spurious waves that travel at different speeds will lead to a
spatially nonhomogeneous wave field with the wave height changing continuously over the
domain.
For this unwanted situation, it is recommended to add second order bound waves at the
wavemaker boundary so to avoid the presence of spurious waves. When a monochromatic wave is
to be imposed at the open boundary, then bound super-harmonic wave components derived from
the second order Stokes pertubation expansions (Vasarmidis et al., 2024) can be added, while for
a bichromatic wave and a spectral wave also the bound sum- and difference-frequency
components are included at the wavemaker boundary. This can be achieved by the command
ADDBoundwave.
Like the dispersion relation, the solution to the second order Stokes wave theory is derived by
means of the Keller-box scheme (see Section 5.4.3) and also depends on the number of
equidistant layers employed in the model. It is limited up to four layers. For details, we refer to
Vasarmidis et al. (2024).
The second order Stokes corrections are derived with the assumption of weak nonlinearity. This
implies that the proposed boundary condition cannot be used in the surf zone (a∕d ∼ 1) and in
deep water (kd > 1). This is the case when the Ursell number a∕d∕ (kd)3 exceeds 0.2. In that
case, SWASH will give a warning. Nevertheless, for most practical applications, the boundary
will be located in intermediate water depths where these limitations are not met. Furthermore, in
deep water the second order response is small and can − to a good approximation − be
neglected. In such case, a boundary condition based on linear wave theory is likely
sufficient.
To simulate entering waves without some reflections at the wavemaker boundary, a weakly
reflective condition allowing outgoing waves must be adopted (command BTYPE WEAK). This
type of radiation condition has been shown to lead to good results within the surf
zone.
Waves propagating out of the computational domain are absorbed by means of a sponge layer
placed behind an output boundary. It is recommended to take the width of the sponge layer at
least 3 times the typical wave length. However, for long waves a Sommerfeld radiation condition
might be a good alternative.
When no boundary conditions are specified at a boundary, this boundary is considered to be a closed one. This boundary is fully reflective. Alternatively, periodic boundary conditions can be applied at two opposite boundaries. This means that wave energy leaving at one end of the domain enters at the other side. In this case no reflections at these boundaries occur. This is recommended in the case of a simulation of a field case where longshore bottom variations are negligible. In such a case the computational domain is made repeated in a representative direction (see command CGRID ... REPeating X|Y).
It is recommended to take into account both the spin up time and the duration of
the time series at the wavemaker boundary. In this way, a steady-state condition will
be obtained. We assume that the spin up time takes at most 10 to 15% of the total
time of the simulation. For a suitable simulation time at least 500 to 1000 waves are
needed.
In the above example the cycle period equals 30 minutes, which is supposed to be at least 85% of the total simulation time. So, the duration of the intended simulation would be 35 minutes, or more safely, 40 minutes.
The time integration is of explicit type and thus requires strict confirmity of stability criteria for a stable solution. The well-known CFL condition for 1D problems is given by
| (5.1) |
with Δx the mesh width, Δt the time step, u the flow velocity, and Cr the Courant number. For a 2D problem, however, the following CFL condition is employed
A dynamically adjusted time step controlled by the Courant number in a user prescribed range is implemented in SWASH as follows. The actual maximum of the Courant number over all wet grid points is determined. The time step is halved when this number becomes larger than a preset constant Crmax < 1, and the time step is doubled when this number is smaller than another constant Crmin, which is small enough to be sure the time step can be doubled. Usually, Crmin is set to 0.2, while the maximum Courant number Crmax is specified in the range of 0.5 to 0.8. It is advised not to choose a value higher than 0.8 since nonlinear processes, e.g. wave breaking and wave-wave interactions, can affect the stability condition. For high, nonlinear waves, or wave interaction with structures with steep slopes (e.g. jetties, quays), a Courant number of 0.5 is advised.
Spatial discretization of the governing equations is carried out in a finite volume/finite difference fashion. A staggered grid arrangement is used in which the velocity components are located at the center of the cell faces (see Figure 5.2). The water level is located at cell center. Concerning the non-hydrostatic pressure, two layouts to assign this unknown to grid points are employed. This variable can be given either at the cell center or at the layer interface. The former is called the standard layout, while the latter one is called the box layout; see Figure 5.2.
The choice depends on the discretization of the vertical pressure gradient, namely, explicit
central differences referring as the classical case and the implicit Keller-box or compact scheme,
respectively. This compact scheme allows straightforward implementation of the zero pressure
boundary condition at the free surface without the need for special attention at interior points
near that surface. Moreover, the discretization error is four to six times smaller than the error of
classical central differences of the same order and involving the same number of vertical grid
points. Hence, use of the compact scheme allows a very few number of vertical grid
points with relative low numerical dispersion and dissipation, thereby enhancing the
accuracy of the frequency dispersion for relative short waves up to an acceptable level, see
Table 5.1.
At very low vertical resolution (one or two layers), the Keller-box scheme gives good dispersive
properties. At high vertical resolutions, however, the standard layout is preferable because it
appears to be more robust while its dispersion characteristics are then usually sufficiently
accurate.
To summarize, for wave simulations with 5 layers or less, the Keller-box scheme using the box
layout is recommended, while for simulations with typically 10−20 layers, the classical central
differencing employing the standard layout is preferred. See command NONHYDrostatic
STANdard|BOX.
Related to this choice, it might be useful to specify the preconditioner for solving the Poisson pressure equation. Two options are available: ILU and ILUD. For a robust solution, the ILU preconditioner is preferred. This choice might be a good one for applications where high and short waves are involved, or irregular beds with steep slopes (e.g. weir, breakwater, quay, jetty), or when relatively large number of layers (> 30) are involved. On the other hand, the ILUD preconditioner is a better choice to get an efficient solution (e.g. parallel computing). See command NONHYDrostatic ... PREConditioner ILUD|ILU.
For simulation of breaking waves, hydraulic jumps and bores, momentum must be conserved. Preference should then be given to a numerical method that conserves momentum, which ensures that the wave properties under breaking waves are modelled correctly. See command DISCRET UPW MOM.
We make a distinction between horizontal and vertical advection terms of the momentum equations. Moreover, we consider the momentum equations separately, i.e. the u−momentum equation and the w−momentum equation. Note that the v−momentum equation will be treated as the u−momentum equation in exactly the same way. So, we have four different commands:
Below, they will be outlined, respectively.
Horizontal advection terms of u−momentum equation
We consider terms like
There are many schemes to approximate these terms. Some of these schemes are accurate but
are prone to generate wiggles − typically space-centred schemes. Other schemes generate a
certain amount of numerical diffusion and thus may affect the wave amplitude or wave
energy of particularly short waves − typically upwind schemes. Higher order upwind
schemes still generate small wiggles. If this is not desired, a flux-limiting scheme may be
employed instead. Upwind schemes are known to be more stable than space-centred
approximations.
The default scheme for the considered terms is the well-known second order BDF scheme (or
sometimes called the LUDS scheme). For many applications this is a good choice. However, in
some cases central differences (CDS) are preferred. This is especially the case when the higher
harmonics are involved or when wave breaking is present (the amount of dissipation of higher
harmonics is then important). Note that when the command BREAK is employed, SWASH will
automatically apply central differences to the horizontal advection terms. If, for some reason,
SWASH becomes unstable, possibly due to the growth of wiggles, the user is then advised to use
the BDF scheme.
Other higher upwind schemes (e.g. QUICK) may be used as well, but we did not experience
much differences compared to the BDF scheme. In any case, never apply the first order
upwind scheme to any horizontal advection term, which is usually too numerically
diffusive.
Horizontal advection terms of w−momentum equation
The horizontal advection terms of the w−momentum equation are given by
These terms are usually ignored. For some applications they are negligible small compared to the vertical pressure gradient. However, they will be automatically taken into account in the simulation for
If they are included, then the second order BDF scheme will be employed. Sometimes, central
differences are preferred, for instance, when the higher harmonics are involved.
Vertical advection term of u−momentum equation
The vertical advection term of the u−momentum equation reads
This term is only included in the computation when more than one layer is chosen (K > 1). The
default scheme for this advection term is the MUSCL scheme. However, when many layers are
involved or higher harmonics are present, then central differences might be a better
choice.
Vertical advection term of w−momentum equation
This term is given by
and is usually ignored even when K > 1 (for an explanation, see Section 5.3). It will be included automatically if the vertical flow structure is present (the standard layout for non-hydrostatic pressure is employed). This term is by default approximated with the MUSCL scheme.
For the calculation of wave runup and rundown on the beach, use of a moving boundary condition is required. The method used in SWASH to track the moving shoreline amounts to ensure non-negative water depths. For a one-dimensional case, one can show that if
and if a first order upwind scheme is applied to the global continuity equation, we
shall have non-negative water depths at every time step; see [2] for a proof. Hence,
flooding never happens faster than one grid size per time step, which is physically
correct. This implies that the calculation of the dry areas does not need any special
feature. For this reason, no complicated drying and flooding procedures are required.
Additionally, the shoreline motion in the swash zone can be simulated in a natural
manner.
For computational efficiency, the model equations are not solved and the velocities are set to zero
when the water depth is below a threshold value (see command SET DEPMIN). Its default value is
0.05 mm. However, a higher threshold value may be chosen for scaling reasons. For instance,
at the scale of a field site, a value of 1 mm is an appropriate choice. (As a matter
of fact, the value of 0.05 mm is a suitable one under laboratory conditions.) This
will also relax the time step to some extent in case of explicit time stepping. For a
large-scale ocean simulation, a threshold value of 1 cm is probably more effective than 0.05
mm. Be careful when choosing a too high value as this may negatively influence mass
conservation.
To achieve second order accuracy, the so-called MUSCL limiter may be employed (see command
DISCRET CORRDEP).
Since the CFL condition, Eq. (
), holds this implies that ensuring non-negative water depths
does not lead to a new time step restriction.
For some two-dimensional cases, however, ensuring non-negative water depths might lead to a time step restriction which appears to be more restrictive than the usual CFL condition. An example is the case where locally all velocities are directed outward of a grid cell. Nevertheless, such a case is rarely encountered and usually the time step is restricted by the Courant number based on the stability criterion.
Neither Boussinesq-type wave models nor non-hydrostatic wave-flow models can be directly
applied to details of breaking waves, since in both models essential processes such as overturning,
air-entrainment and wave generated turbulence, are absent. But, if only the macro-scale effects of
wave breaking are of interest, such as the effect on the statistics of wave heights, details of the
breaking process can be ignored. By observing that both spilling and plunging breakers
eventually evolve into a quasi-steady bore, where the entire front-face of the wave is turbulent, a
breaking wave becomes analogous to a hydraulic jump. Consequently, its integral properties (rate
of energy dissipation, jump height) are approximately captured by regarding the breaking wave
as a discontinuity in the flow variables (free surface, velocities). Proper treatment of such a
discontinuity in a non-hydrostatic model (conservation of mass and momentum) can
therefore be used to determine the energy dissipation of waves in the surf zone; see
Section 5.4.4.
Though a vertical coarse resolution (1−3 layers) is sufficient to describe the wave physics outside
the surf zone (e.g. refraction, shoaling, diffraction, nonlinear wave-wave interactions), dissipation
due to wave breaking requires a disproportional high vertical resolution (∼10−20). A coarse
resolution will result in an underestimation of the horizontal velocities near the wave crest, and
thus an underestimation of the amplitude dispersion. This underestimation implies that at low
vertical resolution the influence of the non-hydrostatic pressure gradient is overestimated.
Consequently, the stabilizing dispersive effects (i.e. the non-hydrostatic pressures) postpone
the transition into the characteristic saw-tooth shape and therefore also the onset of
dissipation.
By enforcing a hydrostatic pressure distribution at the front of a wave, we can locally reduce a
non-hydrostatic wave-flow model to the nonlinear shallow water equations. The wave then
rapidly transitions into the characteristic saw-tooth shape and, consistent with the high
resolution approach, dissipation is captured by ensuring momentum conservation over the
resulting discontinuity.
The subsequent dissipation is well described by assuming depth uniform velocities and a
hydrostatic pressure distribution. In fact, these assumptions often form the basis to derive
dissipation formulations to account for depth-induced breaking in energy balance type models,
e.g. Battjes and Janssen (1978) among many others. Hence, prescribing a hydrostatic pressure
distribution in the model around the discontinuity should result in the correct bulk
dissipation.
There is no need to assume a hydrostatic pressure distribution if the vertical resolution is
sufficient (i.e. 10 to 20 layers). However, imposing a hydrostatic distribution resolutions at low
resolutions (1−3 layers) will ensure that, due the absence of dispersive effects, the front
quickly transitions into a bore like shape. Hence, it can be used to initiate the onset of
wave breaking, thus allowing for the use of low-vertical resolutions throughout the
domain. In practice this means that once a grid point is in the front of a breaking wave,
vertical accelerations are no longer resolved, and the non-hydrostatic pressure is set to
zero.
A grid point is therefore labelled for hydrostatic computation if the local surface steepness ∂ζ∕∂x
exceeds a predetermined value α. Equivalenty, ∂ζ∕∂t > α
. Once labelled, a point only
becomes non-hydrostatic again if the crest of the wave has passed. This is assumed to occur
when ∂ζ∕∂t < 0. Furthermore, because grid points only become active again when the crest
passes (where w ≈ 0), vertical velocities w are set to zero on the front. To represent persistence
of wave breaking, we locally reduce the criterion α to β if a neighbouring grid point (in x− or
y−direction) has been labelled for hydrostatic computation. In this case a point is thus also
labelled for hydrostatic computation if ∂ζ∕∂t > β
, with β < α. In all other grid points,
the computations are non-hydrostatic. Based on calibration, the default value for the
maximum steepness parameter α is 0.6, while the persistence parameter β is set to
0.3.
To summarize, in case of a few layers (1−3) we must apply the command BREAK with optionally different values for α and β. In case of a sufficient number of layers (>10) nothing needs to be specified with respect to wave breaking.
In case of the lateral mixing of momentum, e.g. around the tips of breakwaters and dams, it is recommended to employ the well-known Smagorinsky subgrid model in which the mixing length is assumed to be proportional to the typical grid spacing. The default value for the Smagorinsky constant is 0.2.
If the user is interested in the vertical flow structure, it is advised to apply the standard k − 𝜀 turbulence model in order to take into account the vertical mixing. For stability reason, a background viscosity of 0.0001 m2∕s is recommended (see command SET [backvisc]).
When waves are travelling over a relatively long distance of order of several kilometres, the influence of bottom friction becomes more pronounced. Moreover, it may affect long waves close to the shoreline, e.g. infragravity waves, and nearshore circulations. For wave simulations, a Manning coefficient of 0.019 is recommended.
SWASH calculates the time-dependent evolution of the surface elevation, velocities (both
horizontal and vertical), pressure and possibly some turbulence quantities. It would
require an excessive amount of disk space to the store these quantities at every grid
point for every time step. Therefore, the user has to make some decisions on what
need to be outputted by SWASH. One can make some tables of time series of surface
elevation, velocities, discharges, pressures, turbulent kinetic energy, etc. or time-averaged
velocities and turbulence quantities or wave height and wave-induced setup at specified
location points. Alternatively, one may also output several quantities over the entire
domain or a part of the domain at certain times (”snapshots”). They are stored as
blocks in the Matlab binary files. Note that the corresponding file size is limited to 8
GB.
The user must determine the time duration over which the wave parameters, e.g. wave height and setup, mean current or mean turbulence quantities are computed; see command QUANT. This corresponds to the final stage of the simulation period, which should be long enough to establish steady-state conditions. This time duration, which should be long enough to provide statistically reliable data, equals the duration of the simulation minus the spin up time of the simulation; see Section 5.4.1.
Suppose one wants to simulate a harbour with a typical domain size of 2 × 2 km2 with SWASH. In addition, we assume the following typical values:
According to the dispersion relation, kd = 1.4 or the wave length of the primary wave is about 90 m.
We choose a grid size of 2 m, being 1/45 of the wave length. Requiring a wave Courant number
of at most 0.5, the associated time step is 0.03 s. To take into account the higher harmonics in
the simulation accurately, two layers will be chosen (see Table 5.2; the minimum wave period is
3.2 s, which is 2.5 times smaller than the peak period of 8 s). On a present-day computer (2.0
GHz Intel Core 2 processor) SWASH requires about 6 μs per grid point and per time step for a
two-layer simulation. So, the simulation of our harbour takes about 17 days on a single processor
to complete the run of 60 minutes real time. This clearly shows the need for parallel
computing.
Different parallelization strategies can be considered of which the most popular are:
Data parallel programming uses automatic parallelizing compilers which enables loop-level
parallelization. Generally, this approach often will not yield high efficiency. The main
reason for this is that a large portion of the existing code is in most cases inherently
sequential.
On shared memory platforms with all processors using a single memory, parallelization is usually
done by multithreading with the help of OpenMP compiler directives. A drawback of this
approach is that forcing good parallel performance limits the number of processors only to about
16.
Obtaining good scalability for relatively large number of processors is usually achieved through
distributed memory parallel machines with each processor having its own private memory. A
popular example of distributed memory architecture is a cluster of Linux PCs connected via fast
networks, since it is very powerful, relatively cheap and nearly available to all end-users. The
conventional methodology for parallelization on distributed computing systems is domain
decomposition, which not only achieves benefit from carrying out the task simultaneously on
many processors but also enables a large amount of memory required. It gives efficient
parallel algorithms and is easy to program within message passing environment such as
MPICH2.
A parallel version of SWASH with the distributed memory parallelization paradigm
using MPI standard has been developed. The message passings are implemented by a
high level communication library MPICH2. Only simple point-to-point and collective
communications have been employed. No other libraries or software are required. For a
full three-dimensional simulation with a high resolution we expect a good scalable
performance.
Refer to the example above, numerical computations have been carried out for the full simulation period of our harbour on 1 through 32 computational cores of our Linux cluster. The results show a super linear speedup of up to a factor 8.6 on 8 cores, but then it levels off to a factor of 26 on 32 cores. As such, the computing time has been reduced to 15 hours per 60 minutes to be simulated.
In SWASH a number of variables are used in input and output. The definitions of these variables are mostly conventional.
![Hs Significant wave height, in meters, de fined as
∘ ∫--------
Hs = 4 E(f )df
where E(f ) is the variance density spectrum and f is the frequency.
With respect to output, this quantity is computed as four times the
standard deviation of the surface elevation over the duration [dur ]
(see command QUANTITY ) in the final stage of the simulation, which
should be long enough to provide statistically reliable wave height.
The simulation period should therefore be long enough to establish
steady-state conditions.
Hrms RMS wave height, in meters, defined as
√ --
Hrms = 12 2Hs
T Peak period, in seconds, defined as inverse of the frequency at which
p
the variance density spectrum is a maximum.
Tm01 Mean wave period, in seconds, defined as
∫
∫-E(f)df-
Tm01 = fE (f)df
Directional spread The directional distribution of incident wave energy is given by
m
D (𝜃) = A cos (𝜃) for all frequencies. The power m is related to
the one-sided directional spread as given in Table A.1.
Cr Courant number defined as follows:
(√ --- √ -------) ∘ -1-----1--
Cr = Δt gd + u2 + v2 Δx2-+ Δy2
with Δt the time step, Δx and Δy the grid sizes in x− and y− direction,
respectively, and u and v the velocity components in x − and y− direction.
VEL Current velocity components in x− and y− direction of the problem
coordinate system, except in the case of output with BLOCK command in
combination with command FRAME, where x and y relate to the x− axis
and y − axis of the output frame.
MVEL Mean or time-averaged velocity components in x− and y− direction of
the problem coordinate system, except in the case of output with BLOCK
command in combination with command FRAME, where x and y relate
to the x− axis and y− axis of the output frame. Time -averaging is carried
out over the duration [dur ] (see command QUANTITY ) in the final stage
of the simulation.
WIND Wind velocity components in x − and y− direction of the problem
coordinate sytem, except in the case of output with BLOCK command in
combination with command FRAME, where x and y relate to the x− axis
and y − axis of the output frame.
TIME Full date-time string.
TSEC Time in seconds with respect to a reference time (see command QUANTITY ).
Cartesian convention The direction is the angle between the vector and the positive x− axis,
measured counterclockwise. In other words: the direction where the
waves are going to or where the wind is blowing to.
Nautical convention The direction of the vector from geographic North measured
clockwise. In other words: the direction where the waves are coming
from-or where the wind is blowing from.](swashuse186x.svg)
| m | directional spread (in o) |
| 1. | 37.5 |
| 2. | 31.5 |
| 3. | 27.6 |
| 4. | 24.9 |
| 5. | 22.9 |
| 6. | 21.2 |
| 7. | 19.9 |
| 8. | 18.8 |
| 9. | 17.9 |
| 10. | 17.1 |
| 15. | 14.2 |
| 20. | 12.4 |
| 30. | 10.2 |
| 40. | 8.9 |
| 50. | 8.0 |
| 60. | 7.3 |
| 70. | 6.8 |
| 80. | 6.4 |
| 90. | 6.0 |
| 100. | 5.7 |
| 200. | 4.0 |
| 400. | 2.9 |
| 800. | 2.0 |
The actual commands of the user to SWASH must be given in one file containing all commands. This file is called the command file. It must be presented to SWASH in ASCII. It is important to make a distinction between the description of the commands in this User Manual and the actual commands in the command file. The descriptions of the commands in this User Manual are called command schemes. Each such command scheme includes a diagram and a description explaining the structure of the command and the meaning of the keyword(s) and of the data in the command. The proper sequence of the commands is given in Section 4.2.
Each command instructs SWASH to carry out a certain action which SWASH executes before it reads the next command. A command must always start with a keyword (which is also the name of the command) which indicates the primary function of that command; see list in Section 4.1). A simple command may appear in its command scheme as:
KEYword data
A command may contain more than one keyword (which refines the instructions to SWASH), e.g.,
KEY1word KEY2word data
where KEY2word is the second keyword.
In every command scheme, keywords appear as words in both lower- and upper-case letters.
When typing the command or keyword in the command file, the user must at least copy
literally the part with upper-case letters. SWASH reads only this part. SWASH is case insensitive
except for one instance (character strings), see below. When typing the keyword in the command
file, any extension of the part with upper-case letters is at the users discretion as long as the
extension is limited to letters or digits, as well as the characters − and _. So, in the first
command outlined above one may write: KEY or KEYW or KEY−word or keyhole, etc., whereas
with the abovementioned second command scheme, key1 KEY2 data may appear in the
command file.
In the command file
All keywords in a command are required except when an option is available.
Optional keywords are indicated in the command scheme with the following signs enclosing the keywords concerned:
| KEY1word ...... data ....... | < > | KEY2word ...... data ....... |
For the above example it may appear as:
| KEY2word data | KEY1word < > | KEY3word data |
In case the user does not indicate an option in a command, SWASH chooses the alternative indicated with an arrow (->) appearing in the command scheme (the default option). In the above example, it may appear as:
| KEY2word data | KEY1word < > | -> KEY3word data |
where KEY3WORD is the default option.
The use of keywords is sometimes repetitive, e.g. in a sequence of data and keywords containing many locations in x,y−space. In such a case, the command scheme indicates this repetitive nature by placing the keywords (and data) concerned between angle brackets < >. For instance,
KEY1word <data KEY2word data>
In the actual command in the command file the user must give such a sequence. It ends with either
If more than one line is required for a command, the user may continue on the next line as described in Section B.4. The repetition may consist of one instance (in fact, no repetition at all).
Most commands contain data, either character data or numerical data.
Character data (character strings) are represented in the command schemes by names, enclosed
in quotes (’ ’).
Numerical data are represented in the command schemes by names enclosed in square brackets ([
]).
As a rule, an error message will result if numerical data is given where character data should be given.
Character data are represented as character strings (sequence of characters and blanks) between
quotes (in the command scheme and in the command file). SWASH interprets an end of line as
an end quote (a character data field can therefore never extend over more than one
line).
In a command scheme the character string is always a name (which is placed between quotes as indicated). In the command file such a name can be entered in two ways:
As a rule, an error message will result if numerical data is given where character data should be
given.
Numerical data are simple numbers, e.g. 15 or −7 (integer data), or 13.7 or 0.8E−4 (real data).
Whether or not integer number or real number should be given by the user is indicated in the
description of the command scheme.
Note that a decimal point is not permitted in an integer number. On the other hand, an integer
number is accepted by SWASH where a real number should be given.
In a command scheme, the number is always indicated with a name (which is placed between square brackets). In the command file such a name can be entered in two ways:
All data must be given by the user in the command file in the same order as they appear in the
command scheme. They are separated by blanks or comma’s.
Required data (indicated in the description of each individual command) must be given explicitly
as character string or numbers.
Optional data are indicated
(a)
in the text of each individual command or
(b)
for sets of data: in parenthesis around the data concerned
( data )
For example:
KEY1word KEY2word ’name’ ([nnn] [mmm]) [zzz]
or
(c)
some optional data are indicate in the same way as optional keywords are indicated:
| .....data.....|
< >
| .....data.....|
Optional data of the kind (a) or (b) may be omitted by giving blanks between comma’s (SWASH then substitutes reasonable default values). If after a required datum all data is optional (till the next keyword or the next end-of-line), then the comma’s may be omitted too. Optional data of the kind (c) are to be treated in the same way as optional keywords.
All text after one $ or between two $ signs on one line in the command file is ignored by SWASH as comment. Such comments may be important to the user e.g., to clarify the meaning of the commands used. In fact, this option has been used to create the edit file swash.edt (see Appendix C). Anything appearing after two $ signs is not interpreted as comment, but again as data to be processed (possibly interrupted again by $ or two $ signs). Alternatively, the exclamation mark ‘!’ can be used as comment sign. Everthing behind a ! is interpreted as comment, also if ! or $ are in that part of the input line.
A command in the command file may be continued on the next line if the previous line terminates with a continuation mark & or _ (underscore).
Below the file swash.edt is presented in which all the commands that can be used with SWASH
are specified.
! PROJECT ’name’ ’nr’
! ’title1’
! ’title2’
! ’title3’
!
! SET [level] [nor] [depmin] [maxmes] [maxerr] [seed] &
! [grav] [rhowat] [temp] [salinity] [dynvis] [rhoair] [rhosed] &
! [cdcap] [prmean] [backvisc] [kappa] &
! CORIolis CARTesian|NAUTical [epshu] CC &
! [printf] [prtest] [outlev]
!
! MODE DYNamic / -> TWODimensional \ (SKIPMOMentum) (LINear)
! \ ONEDimensional /
!
! COORDinates / -> CARTesian
! \ SPHErical CCM|QC
!
! | REGular [xpc] [ypc] [alpc] [xlenc] [ylenc] [mxc] [myc] |
! CGRID < CURVilinear [mxc] [myc] (EXC [xexc] [yexc]) > &
! | UNSTRUCtured |
!
! REPeating X|Y
!
! VERTical [kmax] < [thickness] M|PERC >
!
! INPgrid BOT|WLEV|CUR|VX|VY|FRic|WInd|WX|WY|PRessure|POROs|PSIZ|HSTRUC| &
! NPLAnts|DRAFt|LABel|SALinity|TEMPerature|SEDiment|MWL|ACUR| &
! AVX|AVY &
!
! | REG [xpinp] [ypinp] [alpinp] [mxinp] [myinp] [dxinp] [dyinp] |
! | |
! < CURVilinear STAGgered > &
! | |
! | UNSTRUCtured |
!
! (EXCeption [excval]) &
!
! (NONSTATionary [tbeginp] [deltinp] SEC|MIN|HR|DAY [tendinp]) &
!
! (NONUNIForm [kmax])
!
! READgrid UNSTRUCtured / -> TRIAngle \
! \ EASYmesh / ’fname’
!
! READinp BOTtom|WLEVel|CURrent|FRic|WInd|PRessure|COOR|POROs|PSIZ|HSTRUC| &
! NPLAnts|DRAFt|LABel|SALinity|TEMPerature|SEDiment|MWL|ACURrent &
!
! | ’fname1’ |
! [fac] < SERIes ’fname2’ > [idla] [nhedf] ([nhedt]) (nhedvec]) &
! | LAYers ’fname3’ |
!
! FREE | FORMAT ’form’ | [idfm] | UNFORMATTED
!
! | -> CONstant [wlev] [vx] [vy] [tke] [epsilon]
! |
! INITial < ZERO
! |
! | STEAdy
!
!
! | PM |
! BOUnd SHAPespec < -> JONswap [gamma] > SIG|RMS PEAK|MEAN DSPR POW|DEGR
! | TMA |
!
! / -> SIDE N|NW|W|SW|S|SE|E|NE | [k] CCW|CLOCKWise \
! BOUndcond < > &
! \ SEGment / -> XY < [x] [y] > \ /
! \ IJ < [i] [j] > | < [k] > /
!
! BTYPe WLEV|VEL|DISCH|RIEMann|LRIEmann|WEAKrefl|SOMMerfeld|OUTFlow &
!
! LAYer [k] | HYPerbolic | LOGarithmic &
!
! SMOOthing [period] SEC|MIN|HR|DAY &
!
! ADDBoundwave | ADDIG &
!
! | FOURier [azero] < [ampl] [omega] [phase] >
! | REGular [h] [per] [dir]
! | BICHromatic [h1] [h2] [per1] [per2] [dir1] [dir2]
! | UNIForm < SPECTrum [h] [per] [dir] [dd] [cycle] SEC|MIN|HR|DAY
! | | SERIes ’fname’ [itmopt]
! | | SPECFile ’fname’ [cycle] SEC|MIN|HR|DAY
! < &
! | | FOURier < [len] [azero] < [ampl] [omega] [phase] > >
! | | REGular < [len] [h] [per] [dir] >
! | | BICHrom < [len] [h1] [h2] [per1] [per2] [dir1] [dir2] >
! | VARiable < SPECTrum < [len] [h] [per] [dir] [dd] [cycle] S|MI|HR|DA >
! | SERIes < [len] ’fname’ [itmopt] >
! | SPECFile < [len] ’fname’ [cycle] SEC|MIN|HR|DAY >
! | SPECSwan ’fname’ [cycle] SEC|MIN|HR|DAY
!
!
! SOURce X|Y | [k] [centre] [width] [depth] [delta] &
!
! / REGular [h] [per] [dir] \
! \ SPECTrum [h] [per] [dir] [dd] [cycle] SEC|MIN|HR|DAY / &
!
! SMOOthing [period] SEC|MIN|HR|DAY
!
!
! SPONgelayer N|NW|W|SW|S|SE|E|NE [width] | < [k] [width] >
!
!
! FLOAT [alpha] [theta]
!
!
! BODY DIMension [l] [mass] [Ix] [Iy] [Iz] [cogx] [cogy] [cogz] &
!
! DOF SUrge SWay HEave ROll PItch YAw &
!
! ( MLIne < [K] [B] [apbx] [apby] [apbz] [apfx] [apfy] [apfz] [elen] > &
!
! PRETension ) &
!
! ( FENder < [K] [apfx] [apfy] [apfz] > )
!
!
! | NEWmark [beta] [gamma] |
! | |
! | -> CH [rho] |
! BODY SOLVer < > COUPling [tol] [maxiter] [relax] &
! | HHT [rho] |
! | |
! | WBZ [rho] |
!
! KBC [theta]
!
!
! | -> CONstant [cd] |
! | |
! | CHARNock [beta] [height] |
! | |
! | LINear [a1] [a2] [b] [wlow] [whigh] |
! | |
! | WU | | REL [alpha]
! WIND [vel] [dir] < > <
! | GARRatt | | RELW [crest]
! | |
! | SMIthbanke |
! | |
! | CHEn |
! | |
! | FIT |
!
!
! | LINear [k]
! |
! | CONstant [cf]
! |
! | CHEZy [cf]
! |
! FRICtion < -> MANNing [cf]
! |
! | COLEbrook [h]
! |
! | | -> SMOOTH
! | LOGlaw <
! | ROUGHness [h]
!
!
!
! | -> CONstant [visc]
! |
! | -> Horizontal < SMAGorinsky [cs]
! | |
! | | MIXing [lm]
! |
! |
! VISCosity < Vertical KEPS [cfk] [cfe]
! |
! |
! | | -> LINear
! | FULL KEPS <
! | | NONLinear
!
!
!
! POROsity [size] [height] [alpha0] [beta0] [wper]
!
!
! VEGEtation < [height] [diamtr] [nstems] [drag] > MASS [cm] POROsity Vertical
!
!
! | -> Sec | | -> NONCohesive [size] |
! TRANSP [diff] [retur] < MIn > < > &
! | HR | | COHesive [tauce] [taucd] [erate] |
! | DAy |
!
! [fall] [snum] [ak] DENSity Y|N [alfa] [crsn] [cp] [ek] &
!
! ANTICreep STAndard|SVK|None
!
!
! BREaking [alpha] [beta] [nufac]
!
!
! AMBient [U] [V] [eta] Cell|Stagg [theta]
!
!
! | STAndard |
! | |
! NONHYDrostatic < -> BOX > [theta] &
! | |
! | DEPthaveraged |
!
! SUBGrid [pmax] REDuced [qlay] &
!
! SOLVer [rhsaccur] [initaccur] [maxiter] [relax] [precfq] &
!
! PREConditioner ILUDS|ILUD|ILU|NONE &
!
! PROJection ITERative [tol] [maxiter]
!
!
! | | UMOM MOMentum|HEAD / -> Horizontal |
! | | \ Vertical |
! | UPWind < |
! | | WMOM / -> Horizontal |
! | | \ Vertical |
! | |
! | CORRdep |
! DISCRETization < > &
! | TRANSPort / -> Horizontal |
! | \ Vertical |
! | |
! | MIMEtic |
! | |
! | | -> Umom |
! | ACURrent < |
! | | Wmom |
!
!
! | NONe |
! | |
! | FIRstorder |
! | |
! | HIGherorder [kappa] |
! | |
! | | -> SWEBy [phi] |
! | | |
! | LIMiter < RKAPpa [kappa] |
! | | |
! | | PLKAPpa [kappa] [mbound] |
! | FROmm |
! | |
! | -> BDF | LUDs |
! | |
! < QUIck >
! | |
! | CUI |
! | |
! | MINMod |
! | |
! | SUPerbee |
! | |
! | VANLeer |
! | |
! | MUScl |
! | |
! | KORen |
! | |
! | SMArt |
!
!
! DPSopt MIN|MEAN|MAX|SHIFt
!
!
! | EXPL [cfllow] [cflhig] (EULer) |
! | |
! TIMEI METH < IMPL [thetac] [thetas] & > &
! | |
! | SOLVer [tol] [maxiter] [weight] NEWTon |
!
! VERTical [thetau] [thetaw] [thetat]
!
!
! FRAME ’sname’ [xpfr] [ypfr] [alpfr] [xlenfr] [ylenfr] [mxfr] [myfr]
!
! GROUP ’sname’ SUBGRID [ix1] [ix2] [iy1] [iy2]
!
! CURVE ’sname’ [xp1] [yp1] < [int] [xp] [yp] >
!
! RAY ’rname’ [xp1] [yp1] [xq1] [yq1] &
! < [int] [xp] [yp] [xq] [yq] >
!
! ISOLINE ’sname’ ’rname’ DEPTH|BOTTOM [dep]
!
! POINTS ’sname’ < [xp] [yp] > | FILE ’fname’
!
!
! |...|
! QUANTity < > ’short’ ’long’ [lexp] [hexp] [excv] [ref] &
! |...|
!
! [dur] SEC|MIN|HR|DAY [depth] [delrp] &
!
! [xcom] [ycom] [zcom] [alpobj] &
!
! / -> PROBLEMcoord \
! \ FRAME /
!
! OUTPut OPTions ’comment’ (TABle [field]) (BLOck [ndec] [len])
!
! BLOCK ’sname’ HEAD | NOHEAD ’fname’ (LAY-OUT [idla]) &
! < TSEC|XP|YP|DEP|BOTL|WATL|DRAF|VMAG|VDIR|VEL|VKSI|VETA| &
! PRESS|NHPRES|QMAG|QDIR|DISCH|QKSI|QETA|VORT|WMAG|WDIR|WIND| &
! FRC|USTAR|UFRIC|HRUN|BRKP|ZK|HK|VMAGK|VDIRK|VELK|VKSIK| &
! VETAK|VZ|VOMEGA|QMAGK|QDIRK|DISCHK|QKSIK|QETAK|PRESSK| &
! NHPRSK|TKE|EPS|VISC|HS|HRMS|SETUP|MVMAG|MVDIR|MVEL|MVKSI| &
! MVETA|MVMAGK|MVDIRK|MVELK|MVKSIK|MVETAK|MTKE|MEPS|MVISC| &
! SAL|TEMP|SED|MSAL|MTEMP|MSED|SALK|TEMPK|SEDK|MSALK|MTEMPK| &
! MSEDK [unit] > &
! (OUTPUT [tbegblk] [deltblk] SEC|MIN|HR|DAY)
!
! TABLE ’sname’ HEAD | NOHEAD | STAB | SWASH | IND ’fname’ &
! < TIME|TSEC|XP|YP|DIST|DEP|BOTL|WATL|DRAF|VMAG|VDIR|VEL|VKSI|VETA| &
! PRESS|NHPRES|QMAG|QDIR|DISCH|QKSI|QETA|VORT|WMAG|WDIR|WIND|FRC| &
! USTAR|UFRIC|HRUN|BRKP|ZK|HK|VMAGK|VDIRK|VELK|VKSIK|VETAK|VZ| &
! VOMEGA|QMAGK|QDIRK|DISCHK|QKSIK|QETAK|PRESSK|NHPRSK|TKE|EPS| &
! VISC|HS|HRMS|SETUP|MVMAG|MVDIR|MVEL|MVKSI|MVETA|MVMAGK|MVDIRK| &
! MVELK|MVKSIK|MVETAK|MTKE|MEPS|MVISC|SAL|TEMP|SED|MSAL|MTEMP| &
! MSED|SALK|TEMPK|SEDK|MSALK|MTEMPK|MSEDK|FORCEX|FORCEY|FORCEZ| &
! MOMX|MOMY|MOMZ|TRAX|TRAY|TRAZ|ROTX|ROTY|ROTZ|PTOP|RUNUP > &
! (OUTPUT [tbegtbl] [delttbl] SEC|MIN|HR|DAY)
!
!
!
! / -> IJ < [i] [j] > | < [k] > \
! TEST [itest] [itrace] POINTS < > ’fname’
! \ XY < [x] [y] > /
!
!
! | -> Sec |
! COMPute [tbegc] [deltc] < MIn > [tendc]
! | HR |
! | DAy |
!
! STOP
[1] P. Smit, M. Zijlema, and G. S. Stelling. Depth-induced wave breaking in a non-hydrostatic, near-shore wave model. Coast. Engng., 76:1–16, 2013.
[2] G. S. Stelling and S. P. A. Duinmeijer. A staggered conservative scheme for every Froude number in rapidly varied shallow water flows. Int. J. Numer. Meth. Fluids, 43:1329–1354, 2003.
[3] G. S. Stelling and J. A. Th. M. Van Kester. On the approximation of horizontal gradients in sigma co-ordinates for bathymetry with steep slopes. Int. J. Numer. Meth. Fluids, 18:915–935, 1994.
[4] G. S. Stelling and M. Zijlema. An accurate and efficient finite difference algorithm for non-hydrostatic free-surface flow with application to wave propagation. Int. J. Numer. Meth. Fluids, 43:1–23, 2003.
[5] M. Zijlema. Computation of free surface waves in coastal waters with SWASH on unstructured grids. Comput. Fluids, 213, 2020. Article 104751.
[6] M. Zijlema and G. S. Stelling. Further experiences with computing non-hydrostatic free-surface flows involving water waves. Int. J. Numer. Meth. Fluids, 48:169–197, 2005.
[7] M. Zijlema and G. S. Stelling. Efficient computation of surf zone waves using the nonlinear shallow water equations with non-hydrostatic pressure. Coast. Engng., 55:780–790, 2008.
[8] M. Zijlema, G. S. Stelling, and P. B. Smit. SWASH: an operational public domain code for simulating wave fields and rapidly varied flows in coastal waters. Coast. Engng., 58:992–1012, 2011.
BLOCK, 43
BODY DIMENSION, 21
BODY SOLVER, 22
BOTCEL, 33
BOUND SHAPE, 16
BOUNDCOND, 17
BREAKING, 29
CGRID, 5
COMPUTE, 46
COORDINATES, 4
CURVE, 37
DISCRETIZATION, 32
FLOAT, 20
FRAME, 35
FRICTION, 24
GROUP, 36
INITIAL, 15
INPAMB, 13
INPGRID, 9
INPTRANS, 11
ISOLINE, 39
MODE, 3
NONHYDROSTATIC, 31
OUTPUT, 42
POINTS, 40
POROSITY, 26
PROJECT, 1
QUANTITY, 41
RAY, 38
READAMB, 14
READGRID COORDINATES, 6
READGRID UNSTRUCTURED, 7
READINP, 10
READTRANS, 12
SET, 2
SOURCE, 18
SPONGE LAYER, 19
STOP, 47
TABLE, 44
TEST, 45
TIME INTEGRATION, 34
TRANSPORT, 28
VEGETATION, 27
VERTICAL, 8
VISCOSITY, 25
WIND, 23