You are here
SELFE 1.5k7 Serial User Manual
 Important symbols used in this manual
 Mandatory input files (needed for all runs):

Optional input files (driven by param.in):
 Initial condition for salinity and temperature (salt.ic, temp.ic, and ts.ic)
 Bottom drag (drag.gr3 or rough.gr3)
 wind (wind.th)
 Time history input (flux.th etc.)
 Space and timevarying time history inputs
 obe.out
 adv.gr3
 Kriging flags (krvel.gr3)
 Min. and max. diffusivity (diffmin.gr3 and diffmax.gr3)
 Surface mixing length: xlsc.gr3
 Lat/long coordinates (hgrid.ll)
 Heat exchange (sflux/)
 Conservation check files (fluxflag.gr3)
 vvd.dat, hvd.mom, and hvd.tran
 Amplitudes and phases of boundary forcings
 Nodal factor and equilibrium arguments
 Hot start input (hotstart.in)
 Bed deformation input (bdef.gr3)
 Output files:
Input files
"!" is used to add comments after actual input (as customary in FORTRAN 90);
np: # of nodes in the horizontal grid;
ne: # of elements in the horizontal grid;
ns: # of sides in the horizontal grid;
nvrt: total # of levels in the vertical grid;
mne_ke: max. # of elements used in local Kriging;
nope: total # of open boundary segments;
ntracers: total # of passive tracers.
Horizontal grid (hgrid.gr3)
In xmgredit grid format.
Here is an example; below are explanations of format with this grid:
hgrid.gr3 ! alphanumeric description 60356 31082 ! of elements and nodes in the horizontal grid !Following is coordinate part: 1 402672.000000 282928.000000 2.0000000e+01 ! node #, x,y, depth ............................................. 31082 331118.598253 112401.547031 2.3000000e01 !last node
! Following is connectivity part:
........................................... 60356 3 26914 30943 26804 !last element

!Following is boundary condition part (needed for hgrid.gr3 only):
3 : Number of open boundaries
95 ! Total number of open boundary nodes
3 ! Number of nodes for open boundary 1
29835 ! first node on this segment
29834 ! 2nd node on this segment
29836 ! 3rd node on this segment
90 !Number of nodes for open boundary 2
........................................
2 ! last node on this open segment
16 ! number of land boundaries
1743 ! Total number of land boundary nodes (including islands)
753 0 ! Number of nodes for land boundary 1 ('0' means the exterior boundary)
30381 ! first node on this segment
30380
.......................................
1 !last node on this segment
741 0 ! Number of nodes for land boundary 2 ('0' means the exterior boundary)
.......................................
10 1 ! Number of nodes for island boundary 1 ('1' means island)
29448 ! first node on this island
29451
29525
.......................................
29449 !last node on this island (which is different from the first node above)
.......................................
Note: (1) the boundary condition (b.c.) part can be generated with xmgredit5 > GridDEM > Create open/land boundaries;
(2) if you have no open boundary, you can create two land boundary segments that are linked to each other;
(3) although not required, we recommend you follow the following convention when genrating the boundary segments. For the exterior boundary (open+land), go in counterclockwise direction; for interior boundaries (islands), go in clockwise direction;
(4) The use of a Shapiro filter places some constraints on the boundary sides. In particular, the center of any internal sides must be inside the quad formed by the centers of its 4 adjacent sides (see Fig. 1). If not, the code will try to enlarge the stencil, but if the side is near the boundary, fatal error will occur. To find out all violating boundary elements, just prepare hgrid.gr3 (note that the open boundary info needs no be correct at this stage), vgrid.in and param.in up to ihorcon, and run the code with ipre=1 in param.in. You'll find a list of all such sides in fort.11 (the two node numbers of a side will be shown). Method to eliminate this problem includes: (1) move node, (2) swap the side for a pair of elements, and (3) refine or coarsen. Note that in most grid editors, the first 2 methods won't change the node numbering and so you'd try them first before Method (3), to save time. After the preprocessing run is successful (with a screen message indicating so), you can then proceed to prepare other inputs.
Vertical grid (vgrid.in)
This version uses hybrid SZ coordinates in the vertical, with S on top of Z.
54 18 100. !nvrt; kz (# of Zlevels); h_s (transition depth between S and Z)
Z levels !Zlevels first
1 5000. !level index, zcoordinates
2 2300.
3 1800.
4 1400.
5 1000.
6 770.
7 570.
8 470.
9 390.
10 340.
11 290.
12 240.
13 190.
14 140.
15 120.
16 110.
17 105.
18 100. !
S levels !Slevels below
30. 0.7 10. ! constants used in Scoordinates: h_c, theta_b, theta_f (see notes below)
18 1. !first Slevel (Scoordinate must be 1)
19 0.972222 !levels index,
20 0.944444
.......
54 0. !last
Notes:
 Origin of the vertical axis is at MSL;

h_c, theta_b, theta_f: constants used in Song and Haidvogel's (1994) Scoordinate system. h_c controls surface/bottom boundary layer thickness that requires fine resolution; theta_f>0 leads to traditional sigmacoordinates, while theta_f >> 1 skews resolution towards surface and/or bottom; theta_b=1 leads to both bottom and surface being resolved, while theta_b=0 resolves only surface.  Global output is from the bottom (variable in space) to surface (level nvrt) at each node;
 If a "pure S" model is desired, use only 1 Zlevel and set h_s to a very large number (e.g., 1.e6).
Explanation of each line:

48character string description of the version.

48character start time info string, e.g., 04/23/2002 00:00:00 PST (only used for visualization with xmvis)

ipre: preprocessing flag. ipre=1: code will output centers.bp, sidecenters.bp, obe.out (centers build point, sidcenters build point, and list of open boundary elements), and mirror.out and stop. This is useful also for checking zlevels at various depths (in mirror.out) for any given choice of vgrid. ipre=0: normal run.

nscreen = screen output on/off switch (0: off; 1: on). In either case, mirror output messages will be directed into mirror.out.

iwrite: writing destination option for COIRE system. Default: 0.

imm: tsunami option. Default: 0 (no bed deformation); 1: with bed deformation (needs bdef.bp).

If imm=1, this line is ibdef: total # of deformation steps (i.e., the bed will change from the initial position to the position specified in bdef.bp in ibdef steps).

ihot = hot start flag. If ihot=0, cold start; if ihot/=0, hot start from hotstart.in. If ihot=1, the time and time step are reset to zero, and outputs start from T=0 accordingly. If ihot=2, the run (and output) will continue from the time specified in hotstart.in.

ics = coordinate frame flag. If ics=1, Cartesian coordinates are used; if ics=2, degrees latitude/longitude are used (but the output will still be in Cartesian coordinates).

slam0, sfea0 = centers of projection used to convert lat/long to Cartesian coordinates. These are used for ics=2, or a variable Coriolis parameter is employed (ncor=1), or the heat exchange submodel is invoked (ihconsv=1).

ihorcon: flag to use nonzero horizontal viscosity. If
ihorcon=0, it is not used (recommended). 
theta0 = implicitness parameter (between 0.5 and 1). Recommended value: 0.6.

ibcc, ibtp = barotropic/baroclinic flags. If ibcc=0, a baroclinic model is used and regardless of the value for ibtp, the transport equation is solved. If ibcc=1, a barotropic model is used, and the transport equation may (when ibtp=1) or may not (when ibtp=0) be solved; in the former case, S and T are treated as passive tracers.

If ibcc=0, the next line is:

rnday = total # of run days.

nramp, dramp = ramp option for the tides and some boundary conditions, and rampup period in days (not used if nramp=0).

dt = time step (in sec).

Inactive (will be removed eventually).

nadv = advection on/off switch. If nadv=0, advection is selectively turned off based on the input file adv.gr3. If nadv=1 or 2, advection is on for the whole domain, and backtracking is done using either Euler or 5thorder RungeKutta (expensive) scheme . 
dtb1, dtb2: substeps used in btrack. For nadv /= 0, only dtb1 is used, which is the minimum substep used in Euler scheme (nadv=1) or maximum substep used in 5thorder RungeKutta scheme (nadv=2) For nadv=0, dtb1 is the minimum substep used in Euler scheme (when local depth=1 in adv.gr3) and dtb2 is the maximum substep used in 5thorder RungeKutta scheme (when local depth=2 in adv.gr3) .

h0 = minimum depth (in m) for wetting and drying (recommended value: 1cm). When the total depth is less than h0, the corresponding nodes/sides/elements are considered dry. It should always be positive to prevent underflow.

nchi = bottom friction option. If nchi=0, spatially varying drag coefficients are read in from drag.gr3 (as depth info). For nchi=1, bottom roughnesses (in meters) are read in from rough.gr3. In all cases, the logarithmic law is assumed.

If nchi=1, the next line is: Cdmax = max. drag coefficient (to prevent exaggeration of drag coefficient in shallow areas).

ncor = Coriolis option. If ncor=0 or 1, a constant Coriolis parameter is used (see next line). If ncor=1, a variable Coriolis parameter, based on a betaplane approximation, is used, with the lat/long. coordinates read in from hgrid.ll. In this case, the center of CPP projection must be correctly specified (see above).

If ncor=0, the next line is: cori = constant Coriolis parameter.
If ncor=1, the next line is the reference lattitude in degrees. 
nws, wtiminc = wind forcing options and the interval (in seconds) with which the wind input is read in. If nws=0, no wind is applied (and wtiminc becomes immaterial). If nws=1, constant wind is applied to the whole domain at any given time, and the time history of wind is input from wind.th. If nws=2 or 3, spatially and temporally variable wind is applied and the input consists of a number of netcdf files in the directory sflux/.
The option nws=3 is only for checking heat conservation and needs sflux.th. 
If nws>0, the next two line are: (1) nrampwind, drampwind = ramp option and period (in days) for wind.
(2) iwindoff: option to scale the wind If iwindoff=0, wind is applied as is. If iwindoff=1, the scaling factors are the depths in windfactor.gr3. 
ihconsv, isconsv = heat budget and salt conservation models flags. If ihconsv=0, the heat budget model is not used. If ihconsv=1, a heat budget model is invoked, and a number of netcdf files for radiation flux input are read in from he directory sflux/.
If ELM option is used for heat transport (see iupwind_t below), this is only used to invoke Zeng's bulk aerodynamic model, and the heat budget model is bypassed in the code. If isconsv=1, the evaporation and precipitation model isevoked but the user needs to turn on the preprocessing flag PREC_EVAP in Makefile and recompile. 
itur = turbulence closure model selection. If itur=0, constant diffusivities are used for momentum and transport (and the values are specified in the next line). If itur=2, vertically homogeneous but horizontally varying diffusivities are used, which are read in from hvd.mom.and hvd.tran.
If itur=1, horizontally homogeneous but vertically varying diffusivities are used, which are read in from vvd.dat. If itur=2, the zeroequation Pacanowski and Philander closure is used. If itur=3, then the twoequation closure schemes (MellorYamadaGalperin, Kepsilon, Umlauf and Burchard etc.) are used. If itur=4, GOTM turbulence model is invoked (recommended). 
If itur=0, the next line is: vdiff, tdiff = constant diffusivities for momentum and transport.
If itur=2, the next line is: hestu_pp, vdmax1, vdmin1, tdmin1, hcont_pp, vdmax2, vdmin2, tdmin2. Eddy viscosity is computed as: vdiff=vdiff_max/(1+rich)^2+vdiff_min, and diffusivity tdiff=vdiff_max/(1+rich)^2+tdiff_min, where rich is a Richardson number. The limits (vdiff_max, vdiff_min and tdiff_min) vary linearly with depth between depths hestu_pp and hcont_pp.
If itur=3, the next line is:
mid, stab: choice of model description ("MY"Mellor & Yamada, "KL"GLS as kkl, "KE"GLS as kepsilon, "KW"GLS as komega, or "UB"Umlauf & Burchard's optimal), and stability function ("GA"Galperin's, or "KC"Kantha & Clayson's for GLS models). In this case, the minimum and maximum viscosity/diffusivity are specified in diffmin.gr3 and diffmax.gr3, and the surface mixing length is specified in xlsc.gr3.
If itur=4, GOTM turbulence model is invoked (recommended). But the user need to compile the GOTM libraries first (see FAQ or README inside GOTM/ for instructions), and turn on
preprocessing flag USE_GOTM in Makefile and recompile. T he minimum and maximum viscosity/diffusivity are still specified in diffmin.gr3 and diffmax.gr3, but xlsc.gr3 is not needed. In addition, GOTM also requires an input called gotmturb.inp. There are some readymade samples for this input in the source code bundle. If you wish to tune some parameters inside, you may consult gotm.net for more details. 
icst = options for specifying initial temperature and salinity field for cold start. If icst=1, a vertically homogeneous but horizontally varying initial temperature and salinity field is contained in temp.ic and salt.ic. If icst=2, a horizontally homogeneous but vertically varying initial temperature and salinity field, prescribed in a series of zlevels, is contained in ts.ic.
For general 3D initial S,T fields, use the hot start option. 
ntip, tip_dp: # of constituents used in earth tidal potential; cutoff depth for applying tidal potential (i.e., it is not calculated when depth < tip_dp).

For k=1, ntip
talpha(k) = tidal constituent name;
jspc(k), tamp(k), tfreq(k), tnf(k), tear(k) = tidal species # (0: declinational; 1: diurnal; 2: semidiurnal), amplitude constants, frequency, nodal factor, earth equilibrium argument (in degrees);
end for;

nbfr = total # of tidal boundary forcing frequencies.

For k=1, nbfr
alpha(k) = tidal constituent name;
amig(k), ff(k), face(k) = forcing frequency, nodal factor, earth equilibrium argument (in degrees) for constituents forced on the open boundary;
end for;

nope: # of open boundary segments;

For j=1, nope
neta(j), iettype(j), ifltype(j), itetype(j), isatype(j) = # of nodes on the open boundary segment j (from hgrid.gr3), b.c. flags for elevation, normal velocity, temperature, and salinity;
if (iettype(j) == 1) !time history of elevation on this boundary
no input in this file; time history of elevation is read in from elev.th;
else if (iettype(j) == 2) !this boundary is forced by a constant elevation
ethconst: constant elevation
else if (iettype(j) == 3) !this boundary is forced by tides
for k=1, nbfr
alpha(k) = tidal constituent name;
for i=1, neta(j)
emo(ietaelem(j,i),k), efa(ietaelem(j,i),k) !amplitude and phase for each node on this open boundary;
end for
end for;
else
if (iettype(j) == 4) !space and timevarying input no input in this file; time history of elevation is read in from elev3D.th; else if (iettype(j) == 0) elevations are not specified for this boundary (in this case the velocity must be specified).
endif
if (ifltype(j) == 0) !nornal vel. not specified
no input needed
else if (ifltype(j) == 1) !time history of discharge on this boundary
no input in this file; time history of discharge is read in from flux.th;
else if (ifltype(j) == 2) !this boundary is forced by a constant discharge
vthconst: constant discharge (note that a negative number means inflow)
else if (ifltype(j) == 3) !vel. is forced in frequency domain
for k=1, nbfr
vmo(j,k),vfa(j,k) !uniform amplitude and phase along each boundary segment
end for;
else if (ifltype(j) == 4) !3D input no input in this file; time history of discharge is read in from uv3D.th; else if (ifltype(j) == 1) !Flanther type radiation b.c. (iettype must be 0 in this case) eta_m0,qthcon(j): mean elevation and discharge on the jth boundary
endif
if (itetype(j) == 0) !temperature not specified
no input needed
else if (itetype(j) == 1) !time history of temperature on this boundary
no input in this file; time history of temperature is read in from temp.th;
else if (itetype(j) == 2) !this boundary is forced by a constant temperature
tthconst = constant temperature
else if (itetype(j) == 3) !keep initial temperature profile
no input is needed
else if(itetype(j) == 1) !open b.c.; nudge to initial condition
tobc: nudging factor (between 0 and 1).
else if(itetype(j) == 4) !3D input no input in this file; time history of temperature is read in from temp3D.th; else if(itetype(j) == 4) ! nudge to 3D time series in temp3D.th
tobc: nudging factor (between 0 and 1).
endif
Salintiy b.c. is similar to temperature:
if (isatype(j) == 0) !salinity not specified
.........
endif

nspool, ihfskip: Global output skips. Output is done every nspool steps, and a new output file is opened every ihfskip steps (and in addition, a hotstart file is output at the same time step if the flag nhstar is turned on below). Therefore the outputs are named as [1,2,3,...]_salt.63 etc.

next 25+ lines are global output (in machinedependent binary) options. The outputs share the same structure. Only the first line is detailed here.

noutge = global elevation output control. If noutge=0, no global elevation is recorded. If noutge= 1, global elevation for each node in the grid is recorded in [1,2,3...]_elev.61 in binary format. The output is either starting from scratch or appended to existing ones depending on ihot.

output options for atmospheric pressure (*pres.61).

output options for air temperature (*airt.61).

output options for specific humidity (*shum.61).

output options for solar radiation (*srad.61).

output options for short wave radiation (*flsu.61).

output options for long wave radiation (*fllu.61).

output options for upward heat flux (*radu.61).

output options for downward flux (*radd.61).

output options for total flux (*flux.61).

output options for evaporation rate (*evap.61). 
output options for precipitation rate (*prcp.61).

output options for wind speed (*wind.62).

output options for wind stresses (*wist.62).

output options for depthaveraged velocity (*dahv.62).


output options for vertical velocity (*vert.63).

output options for temperature (*temp.63).

output options for salinity (*salt.63).

output options for density (*conc.63).

output options for eddy diffusivity (*tdff.63).

output options for eddy viscosity (*vdff.63).


output options for turbulent kinetic energy (*kine.63).

output options for macroscale mixing length (*mixl.63).

output options for z coordinates at each node (*zcor.63). This output will always be there even if the flag is turned off.

output options for horizontal velocity (*hvel.64).

In addition, if you use passive tracers and modified the code (ntracer/=0 etc), the corresponding flags are needed here. 26. output options for test variable (test.60). The user may choose any internal variable by modifying the source code 

nhstar= hot start output control parameter. If nhstar=0, no hot start output is generated. If nhstar=1, hot start output is spooled to it_hotstart every ihfskip time steps, where it is the corresponding time iteration number. If a run needs to be hot started from step it, the user can copy
it_hotstart to hotstart.in, as the code expects the hot start input file to be hotstart.in. 
isolver, itmax1, iremove, zeta, tol = ITPACK solver control parameters.
· If isolver=1, the Jacobian Conjugate Gradient Method is used (recommended);
· If isolver=2, the Jacobian SemiIteration Method is used;
· If isolver=3, the Successive Overrelaxation Conjugate Gradient Method is used;
· If isolver=4, the Successive Overrelaxation SemiIteration Method is used;
Recommended values: isolver=1, itmax1=1000, iremove=0, zeta=5.e6, tol=1.e13.

iflux= parameter for checking volume and salt conservation. If turned on (=1), the conservation will be checked in regions specified by fluxflag.gr3.

lq, int_mom: linear (lq=1) or quadratic (lq=2) interpolation for T, S in backtracking, and linear (
int_mom= 0) or Kriging (int_mom= 1) for interpolating the velocityin backtracking . If lq=0, the option is read in from lqk.gr3 as the depth info. Ifint_mom=1, the depth in krvel.gr3 (0 or 1) will determine the order of interpolation (linear or Kriging). 
h_bcc1: depth thresholds used in calculation of bariclonic force. The force will be evaluated using the pressure Jacobian method when h<= h_bcc1 (otherwise the Zmethod is used where interpolation back to Zplane is done). We usually recommend the
Jacobian method, and in this case, a very large h_bcc1 ( e.g. , 1.e6) can be used. 
islip: option for land b.c. islip=0: free slip; =1: no slip.

inu_st, step_nu, vnh1,vnf1,vnh2,vnf2: nudging flag for S,T, nudging step, parameters for vertical nudging. When inu_st=0, no nudging is done. When inu_st=1, nudge to initial conditions. When inu_st=2, nudge to values specified in temp_nu.in and salt_nu.in, given at an interval of step_nu. For inu_st/=0, the horizontal nudging factors are given in t_nudge.gr3 and s_nudge.gr3 (as depths info), and the vertical nudging factors vary linearly along the depth as: min(vnf2,max(vnf1,vnf)), where vnf=vnf1+(vnf2vnf1)*(hvnh1)/(vnh2vnh1). The nudging factor is the sum of the two.

inactive line.

mmm: order of vertical integration used in calculating the baroclinic pressure gradient for
pressure Jacobian method . Must be between 0 and 3. Use mmm=0 for best efficiency, or higher value for accuracy with significant computational cost. 
idrag: bottom drag option. idrag=1: linear drag formulation; idrag=2: quadratic drag
formulation (default). 
inactive line.

ihhat: wet/dry option. If ihhat=1, the frictionreduced depth will be kept nonnegative to ensure robustness (at the expense of accuracy); if ihhat=0, the depth is unrestricted.

iupwind_t,
iupwind_s: upwind option for T,S. A value of "0" corresponds to EulerianLagrangian transport option (and the interpolation method is determined by lq above), "1" for the massconservative upwind option, and "2" for the higherorder massconservative TVD scheme (which may be expensive especially in shallow region). Note that you cannot combine upwind with TVD for S,T, i.e., iupwind_t+ iupwind_s /=3. 
If the TVD option is invoked for at least one of the variables, then this line is: tvd_mid, flimiter. tvd_mid='AA'; flimiter indicates the choice of flux limiting functions: MM (Minmod); OS (Osher); VL (Van Leer) or SB (Superbee). 
vis_coe1,
vis_coe2: blending factor if indvel=0 (see below), i.e., discontinuous velocity + Shapiro filter option. Use 0. 0. 
shapiro: filter strength if indvel=0 (see below). Recommended: 0.5. 
nkrig, kr_co, decol: preferred # of nodes used in Kriging (<=mnei_kr), choice of generalized covariance function, and decorrelation length (in m) for kr_co=5 (otherwise unused). The local neighborhood for a given node is constructed using multiple tiers of surrounding nodes and so the actual number of nodes used may be less than nkrig. The choices for the generalized covariance function include: 1 (linear f(h)=h); 2 (h^2*log(h)); 3: (cubic h^3); 4 (h^5); 5 (Gaussain; not recommended). See Le Roux (1997) for details. 
rmaxvel: maximum velocity. This is needed mainly for the airwater exchange as the model may blow up if the water velocity is above 20m^2/s.

inunfl: choice of inundation algorithm. inunfl=1 can be used if the horizontal resolution is fine enough (e.g., 10m or less), and this is critical for tsunami simulations. Otherwise use inunfl=0. 
indvel: this is an important flag that determines the method of converting side velocity to node velocity. If indvel=0, the node velocity is allowed to be discontinuous across elements and a Shapiro filter is used to filter out subgrid noises. If indvel=1, an averaging procedure is used instead and the node velocity is continuous across elements. In general, indvel=0 leads to smaller numerical diffusion and dissipation and better accuracy. But without a velocity boundary condition, this option will lead to inferior results. If a velocity b.c. is unavailable, indvel=1 should be used. 
ntr: # of passive tracers as defined in the global module. If ntr>0, additional lines are needed that specify the transport method (upwind or TVD) and horizontal boundary conditions etc. Consult the source code for details. See FAQ for how to interface your own code to SELFE.

Depending on the values of icst (see parameter input file):

If icst = 1, salt.ic and temp.ic take the following build point format:
33 to 0 from outh to TP. !file description
30001 !# of nodes;
1 386380.409604 286208.187634 0.000000 !node #, x, y, initial salinity (or temperature)
2 386460.352736 285995.038877 0.000000
3 386687.720000 286213.590000 0.000000
4 386460.076848 286367.779818 0.000000
5 386678.380000 286483.440000 0.000000
.............. 
If icst = 2, ts.ic takes the following format:
43 !total # of vertical levels;
1 2000. 4. 34. !level #, zcoordinates, temperature, salinity
2 1000. 5. 34.
3 500. 6. 33.
4 200. 7. 32.
5 100. 8. 31.
...........
Bottom drag (drag.gr3 or rough.gr3)
grid !file decription
40000 27918 !# of elements, # of nodes
1 386738.500000 285939.060000 0.004500 !node #, x, y, drag coefficient Cd (for nchi=0) or roughness (in meters; for nchi=1)
2 386687.720000 286213.590000 0.004500
3 386421.090000 286172.160000 0.004500
4 386471.720000 286376.030000 0.004500
5 386678.380000 286483.440000 0.004500
6 386140.190000 286439.220000 0.004500
7 386387.280000 286557.310000 0.004500
8 386209.840000 286676.470000 0.004500
..........
If nws=1 in param.in, a time history of wind speed must be specified in this file:
5. 8.660254 ! x and y components of wind speed @ 0*wtiminc
5. 8.660254
5. 8.660254
.......
Note that the speed varies linearly in time, and the time interval (wtiminc) is specified in param.in.
This includes elev.th, flux.th, temp.th, salt.th, which share same structure. Below is a sample flux.th:
300. 1613.05005 6186.60156 !time (in sec), discharge at the 1st boundary with ifltype=1, discharge at the 2nd boundary with ifltype=1
600. 1611.37854 6208.62549
900. 1609.39612 6232.22314
1200. 1607.42651 6254.24707
1500. 1605.45703 6276.27148
1800. 1603.48743 6298.2959
2100. 1601.3772 6321.89307
2400. 1599.40772 6343.91748
2700. 1597.43811 6365.94141
3000. 1595.46863 6387.96582
3300. 1593.49902 6409.99023
3600. 1591.38879 6433.5874
3900. 1589.41931 6452.94287
4200. 1587.2959 6472.29834
...........
Space and timevarying time history inputs:
These include elev3D.th, uv3D.th, temp3D.th, salt3D.th, which share similar structure. For example, uv3D.th:
for it=1,nt !all time steps
time stamp (in sec);
for i=1,nope !all open boundary segments that have this type of b.c.
for j=1,nond(k) !all nodes on this boundary
node #, (uth(i,j,k),vth(i,j,k),k=1,nvrt);
end for !j
end for !i
end for !it
This file is generated with the preprocessing flag in param.in for debugging purpose only.
3 # of open bnd
Element list:
251 bnd # 1
1 31587
2 31588
3 31589
4 31590
5 31592
6 31595
7 31601
8 31603
9 31605
10 31606
........
4 bnd # 2
1 31583
2 31584
3 31585
4 31586
........
If nadv=0, the advection on/off flags are the "depths" (0: off; 1: Euler; 2: 5th order RungeKutta) in this grid file, which is otherwise similar to hgrid.gr3.
The depth specifies the Kriging option for each node: 0 means no Kriging; 1 means applying Kriging there. The order of the generalized covariance function is specified
in param.in.
The depth specifies the minimum and maximum diffusivity imposed at each node. This is needed to further constraint outputs from the GLS model. We generally recommend a constant value of 1.e6 m^2/s for minimum diffusivity, and 1.e2 m^2/s for maximum diffusivity inside estuaries and 10 m^2/s otherwise. The minimum diffusivity may also be changed locally, e.g., to create a mixing pool near the end of a river.
The depth specifies the surface mixing length used when itur=3. It specifies the portion of surface layer thickness; e.g., 0.5 mean 1/2 of the layer is used as surface mixing length. Recommend value: 0.5.
The depth specifies the way the vertical interpolation is done locally, i.e., along Z or S plane. If the depth=1, it is done along Zplane; if the depth=2, along Splane. We recommend the value of 2 in "pure S" zone, and 1 in SZ zone. You may not use "2" in the SZ zone.
Lat/long coordinates (hgrid.ll)
This file is identical to hgrid.gr3 except the x,y coordinates are replaced by lattitudes and longitudes.
This consists of a suite of input for wind and radiation fluxes found in a subdirectory sflux/. When nws=2, the wind speed and atmospheric pressure are read in from this directory; when ihconsv=1, various fluxes are read in from it as well. The netcdf files for various periods have been precomputed by Mike Zulauf and deposited in a data base.
Conservation check files (fluxflag.gr3)

Mass conservation (fluxflag.gr3)
The "depths" of this grid file divide the whole domain into 3 regions: 0, 1 and 2, where regions "1" and "2" must be adjacent to each other. The total volume and various fluxes in regions "1" and "2" are computed.
vvd.dat, hvd.mom, and hvd.tran

vvd.dat (vgrid.in format):
43 !total # of vertical levels;
1 1.e2 1.e4 !level #, viscosity, diffusivity
2 1.e2 1.e4
3 1.e2 1.e4
......................... 
hvd.mom & hvd.tran (build point format)
hvd.mom !file decription
27918 !total # of nodes
1 386738.500000 285939.060000 0.0045 !node #, x, y, viscosity/diffusivity
2 386687.720000 286213.590000 0.004
..............................................
Amplitudes and phases of boundary forcings
To generate amplitudes and phases for each node on a particular open boundary, see SELFE Utilites.