Skip to content

Latest commit

 

History

History
432 lines (315 loc) · 19.8 KB

INFO_INPUT.md

File metadata and controls

432 lines (315 loc) · 19.8 KB

about the input file input.nml

Consider the following input file as example (corresponds to a turbulent plane channel flow with bubbles and walls at different temperatures). &dns defines a so-called Fortran namelist containing the necessary computational parameters to set a case.

&dns
ng(1:3) = 512, 256, 144
l(1:3) = 6., 3., 1.
gtype = 1, gr = 0.
cfl = 0.95, dtmin = 1.e5, dt_f = -1
is_solve_ns = T, is_track_interface = T
inivel = 'poi'
is_wallturb = T, is_forced_hit = F
nstep = 100000, time_max = 100., tw_max = 0.1
stop_type(1:3) = T, F, F
restart = F, is_overwrite_save = T, nsaves_max = 0
icheck = 10, iout0d = 10, iout1d = 100, iout2d = 500, iout3d = 10000, isave = 5000
cbcvel(0:1,1:3,1) = 'P','P',  'P','P',  'D','D'
cbcvel(0:1,1:3,2) = 'P','P',  'P','P',  'D','D'
cbcvel(0:1,1:3,3) = 'P','P',  'P','P',  'D','D'
cbcpre(0:1,1:3)   = 'P','P',  'P','P',  'N','N'
bcvel(0:1,1:3,1) =  0.,0.,   0.,0.,   0.,0.
bcvel(0:1,1:3,2) =  0.,0.,   0.,0.,   0.,0.
bcvel(0:1,1:3,3) =  0.,0.,   0.,0.,   0.,0.
bcpre(0:1,1:3  ) =  0.,0.,   0.,0.,   0.,0.
bforce(1:3) = 0., 0., 0.
gacc(1:3) = 0., 0., 0.
dims(1:2) = 2, 2
\

Additionally, the &scalar namelist contains the computational parameters for scalar transport (e.g. temperature), while the physical and transport properties of the two phases and the numerical parameters of the two-phase solver are specified in the &two_fluid namelist.

&scalar
inisca          = 'dhc'
cbcsca(0:1,1:3) = 'P','P',  'P','P',  'D','D'
bcsca(0:1,1:3)  =  0.,0. ,   0.,0. ,   1.,0.
ssource         = 0.
\

&two_fluid
inipsi            = 'bub3'
cbcpsi(0:1,1:3)   = 'P','P',  'P','P',  'P','P'
cbcnor(0:1,1:3,1) = 'P','P',  'P','P',  'P','P'
cbcnor(0:1,1:3,2) = 'P','P',  'P','P',  'P','P'
cbcnor(0:1,1:3,3) = 'P','P',  'P','P',  'P','P'
bcpsi(0:1,1:3)    =  0.,0. ,   0.,0. ,   0.,0.
bcnor(0:1,1:3,1)  =  0.,0.,    0.,0.,    0.,0.
bcnor(0:1,1:3,2)  =  0.,0.,    0.,0.,    0.,0.
bcnor(0:1,1:3,3)  =  0.,0.,    0.,0.,    0.,0.
sigma             =  1.
rho12(1:2)        =  1., 1.
mu12(1:2)         =  100., 100.
ka12(1:2)         =  0., 0.
cp12(1:2)         =  0., 0.
beta12(1:2)       =  0., 0.
acdi_gam_factor   =  1., acdi_gam_min = 0.
acdi_eps_factor   =  1.
\
Tip for vim/nvim users Consider adding the following lines in your `.vimrc` file for syntax highlighting of the namelist file: 
if has("autocmd")
  au BufNewFile,BufRead *.nml set filetype=fortran
  au BufNewFile,BufRead *.namelist set filetype=fortran
endif
ng(1:3) = 512, 256, 144
l(1:3) = 6., 3., 1.
gtype = 1, gr = 0.

These lines set the computational grid.

ng(1:3) and l(1:3) are the number of points and domain length in each direction.

gtype and gr are the grid stretching type and grid stretching parameter that tweak the non-uniform grid in the third direction; zero gr implies no stretching. See initgrid.f90 for more details. The following options are available for gtype:

  • 1: grid clustered towards both ends (default)
  • 2: grid clustered towards the lower end
  • 3: grid clustered towards the upper end
  • 4: grid clustered towards the middle
cfl = 0.95, dtmin = 1.e5, dt_f = -1

This line controls the simulation time step.

The time step is set to be equal to min(cfl*dtmax,dtmin), i.e. the minimum value between dtmin and cfl times the maximum allowable time step dtmax (computed every ickeck time steps; see below). dtmin is therefore used when a constant time step, smaller than cfl*dtmax, is required. If not, it should be set to a high value so that the time step is dynamically adjusted to cfl*dtmax. Alternatively, one can force the simulation to advance with a constant time step of arbitrary value, independent of the dtmax evaluation, by changing the value of dt_f from -1 to the desired time step.

is_solve_ns = T, is_track_interface = T

is_solve_ns, if true, enables the solution of the Navier-Stokes momentum equation. It can be set to false when a prescribed velocity field is desired. is_track_interface, if true, enables the two-phase interface advection.

inivel = 'poi'
is_wallturb = T, is_forced_hit = F

These lines set the initial velocity field.

initvel chooses the initial velocity field. The following options are available:

  • zer: zero velocity field
  • uni: uniform velocity field equal to uref ; streamwise direction in x
  • cou: plane Couette flow profile with symmetric wall velocities equal to uref/2; streamwise direction in x
  • poi: plane Poiseuille flow profile with mean velocity uref ; streamwise direction in x
  • iop: same as poi, with the reference frame moving with velocity uref ; streamwise direction in x
  • tbl: temporal boundary layer profile with wall velocity uref ; streamwise direction in x
  • pdc: plane Poiseuille flow profile with constant pressure gradient ; streamwise direction in x
  • log: logarithmic profile with mean velocity uref ; streamwise direction in x
  • hcp: half channel with plane Poiseuille profile and mean velocity uref ; streamwise direction in x
  • hcl: half channel with logarithmic profile and mean velocity uref ; streamwise direction in x
  • hdc: half plane Poiseuille flow profile with constant pressure gradient ; streamwise direction in x
  • tgv: three-dimensional Taylor-Green vortex
  • tgw: two-dimensional Taylor-Green vortex
  • rox: solid body rotation with angular velocity $2 \pi$ ; around the x axis
  • roy: solid body rotation with angular velocity $2 \pi$ ; around the y axis
  • roz: solid body rotation with angular velocity $2 \pi$ ; around the z axis
  • vox: two-dimensional, time dependent serpentine vortex ; around the x axis
  • voy: two-dimensional, time dependent serpentine vortex ; around the y axis
  • voz: two-dimensional, time dependent serpentine vortex ; around the z axis

is_wallturb, if true, superimposes a high amplitude disturbance on the initial velocity field that effectively triggers transition to turbulence in a wall-bounded shear flow.

See initflow.f90 for more details.

is_forced_hit, if true, introduces a homogeneous and isotropic forcing in the domain. See forcing.f90 for more details.

nstep = 100000, time_max = 100., tw_max = 0.1
stop_type(1:3) = T, F, F
restart = F, is_overwrite_save = T, nsaves_max = 0

These lines set the simulation termination criteria and whether the simulation should be restarted from a checkpoint file.

nstep is the total number of time steps.

time_max is the maximum physical time.

tw_max is the maximum total simulation wall-clock time.

stop_type sets which criteria for terminating the simulation are to be used (more than one can be selected, and at least one of them must be T)

  • stop_type(1), if true (T), the simulation will terminate after nstep time steps have been simulated
  • stop_type(2), if true (T), the simulation will terminate after time_max physical time units have been reached
  • stop_type(3), if true (T), the simulation will terminate after tw_max simulation wall-clock time (in hours) has been reached

a checkpoint file fld.bin will be saved before the simulation is terminated.

restart, if true, restarts the simulation from a previously saved checkpoint file, named fld.bin.

is_overwrite_save, if true, overwrites the checkpoint file fld.bin at every save; if false, a symbolic link is created which makes fld.bin point to the last checkpoint file with name fld_???????.bin (with ??????? denoting the corresponding time step number). In the latter case, to restart a run from a different checkpoint one just has to point the file fld.bin to the right file, e.g.: ln -sf fld_0000100.bin fld.bin.

nsaves_max limits the number of saved checkpoint files, if is_over_write_save is false; a value of 0 or any negative integer corresponds to no limit, and the code uses the file format described above; otherwise, only nsaves_max checkpoint files are saved, with the oldest save being overwritten when the number of saved checkpoints exceeds this threshold; in this case, files with a format fld_????.bin are saved (with ???? denoting the saved file number), with fld.bin pointing to the last checkpoint file as described above; moreover, a file log_checkpoints.out records information about the time step number and physical time corresponding to each saved file number.

icheck = 10, iout0d = 10, iout1d = 100, iout2d = 500, iout3d = 10000, isave = 5000

These lines set the frequency of time step checking and output:

  • every icheck time steps the new time step size is computed according to the new stability criterion and cfl (above)
  • every iout0d time steps history files with global scalar variables are appended
  • every iout1d time steps 1d profiles are written (e.g. velocity and its moments) to a file
  • every iout2d time steps 2d slices of a 3d scalar field are written to a file
  • every iout3d time steps 3d scalar fields are written to a file
  • every isave time steps a checkpoint file is written (fld_???????.bin), and a symbolic link for the restart file, fld.bin, will point to this last save so that, by default, the last saved checkpoint file is used to restart the simulation

1d, 2d and 3d outputs can be tweaked modifying files out?d.h90, and re-compiling the source. See also output.f90 for more details.

cbcvel(0:1,1:3,1) = 'P','P',  'P','P',  'D','D'
cbcvel(0:1,1:3,2) = 'P','P',  'P','P',  'D','D'
cbcvel(0:1,1:3,3) = 'P','P',  'P','P',  'D','D'
cbcpre(0:1,1:3)   = 'P','P',  'P','P',  'N','N'
bcvel(0:1,1:3,1) =  0.,0.,   0.,0.,   0.,0.
bcvel(0:1,1:3,2) =  0.,0.,   0.,0.,   0.,0.
bcvel(0:1,1:3,3) =  0.,0.,   0.,0.,   0.,0.
bcpre(0:1,1:3  ) =  0.,0.,   0.,0.,   0.,0.

These lines set the boundary conditions (BC) for velocity and pressure.

The type (BC) for each field variable is set by a row of six characters, X0 X1 Y0 Y1 Z0 Z1 where,

  • X0 X1 set the type of BC for the field variable on the lower and upper boundaries in x
  • Y0 Y1 set the type of BC for the field variable on the lower and upper boundaries in y
  • Z0 Z1 set the type of BC for the field variable on the lower and upper boundaries in z

The four rows correspond to the three velocity components, and pressure, i.e. u, v, w, and p.

The following options are available:

  • P periodic
  • D Dirichlet
  • N Neumann

The last four rows follow the same logic, but now for the BC values (dummy for a periodic direction).

bforce(1:3) = 0., 0., 0.
gacc(1:3) = 0., 0., 0.

These lines set the flow forcing.

bforce, is a constant body force density term in the direction in question (e.g., the negative of a constant pressure gradient) that can be added to the right-hand-side of the momentum equation. The three values correspond to three domain directions. gacc, is a constant acceleration in the direction in question (e.g., gravity) added to the right-hand-side of the momentum equation. The three values correspond to three domain directions.

dims(1:2) = 2, 2

This line sets the grid of computational subdomains.

dims is the processor grid, the number of domain partitions along the first and second decomposed directions (which depend on the selected default pencil orientation). dims(1)*dims(2) corresponds therefore to the total number of computational subdomains. Setting dims(:) = [0,0] will trigger a runtime autotuning step to find the processor grid that minimizes transpose times. Note, however, that other components of the algorithm (e.g., collective I/O) may also be affected by the choice of processor grid.

inisca          = 'dhc'

inisca chooses the initial scalar field (e.g. temperature). The following options are available:

  • zer: zero scalar field
  • uni: uniform scalar field equal to sref
  • cou: plane scalar profile, linear between the wall boundary values
  • dhc: differentially heated cavity, in the x direction

See initflow.f90 for more details.

cbcsca(0:1,1:3) = 'P','P',  'P','P',  'P','P'
bcsca(0:1,1:3)  =  0.,0. ,   0.,0. ,   0.,0.

These lines set the boundary conditions (BC) for the scalar.

The type (BC) is set in cbcsca by a row of six characters, X0 X1 Y0 Y1 Z0 Z1 where,

  • X0 X1 set the type of BC for the scalar on the lower and upper boundaries in x
  • Y0 Y1 set the type of BC for the scalar on the lower and upper boundaries in y
  • Z0 Z1 set the type of BC for the scalar on the lower and upper boundaries in z

The following options are available:

  • P periodic
  • D Dirichlet
  • N Neumann

The corresponding BC values are set in bcsca (dummy for a periodic direction).

ssource         = 0.

This line sets the value of a scalar source, that can be added to the right-hand-side of the scalar transport equation.

inipsi          = 'bub3'

inipsi chooses the initial volume fraction field for phase 1 of the two-fluid system. The following options are available:

  • zer : uniform (zero) volume fraction field
  • uni : uniform (unitary) volume fraction field
  • bub1: planar film (lighter phase)
  • bub2: two-dimensional (lighter phase) bubbles
  • bub3: three-dimensional (lighter phase) bubbles
  • drp1: planar film (heavier phase)
  • drp2: two-dimensional (heavier phase) droplets
  • drp3: three-dimensional (heavier phase) droplets
  • cap-wav-1d: planar small-amplitude capillary wave
  • zalesak-disk: two-dimensional (lighter phase) slotted disk

See two_fluid.f90 for more details. For the bub[1-3] and drp[1-3] initial fields, the position and size of the films/bubbles/droplets can be specified by a spheres.in file, where each line corresponds to an individual spherical/circular/planar bubble/droplet, specifying the cartesian coordinates of its center of mass, and its radius. For example, the following file introduces in the computational domain two bubbles/droplets, the first centered at [x,y,z] = [0.3,1.,0.5] with a radius of 0.25, and the second centered at [1.5,0.6,1.] with radius 0.5.

0.3 1.  0.5 0.25
1.5 0.6 1.  0.5

In the case of a planar film (the one-dimensional limit of the sphere), the radius will represent the film thickness, and the film will be aligned along the X-Y plane.

Finally, if the spheres.in file is not specified, the solver will initialize a single sphere, located at the center of the domain, with a size of 0.25 times the smallest domain length, excluding homogeneous directions for 2D and 1D initializations.

cbcpsi(0:1,1:3)   = 'P','P',  'P','P',  'P','P'
cbcnor(0:1,1:3,1) = 'P','P',  'P','P',  'P','P'
cbcnor(0:1,1:3,2) = 'P','P',  'P','P',  'P','P'
cbcnor(0:1,1:3,3) = 'P','P',  'P','P',  'P','P'
bcpsi(0:1,1:3)    =  0.,0. ,   0.,0. ,   0.,0.
bcnor(0:1,1:3,1)  =  0.,0.,    0.,0.,    0.,0.
bcnor(0:1,1:3,2)  =  0.,0.,    0.,0.,    0.,0.
bcnor(0:1,1:3,3)  =  0.,0.,    0.,0.,    0.,0.

These lines set the boundary conditions (BC) for the volume fraction of phase 1 (cbcpsi) and for the three cartesian components of the interface normal (cbcnor).

The type (BC) is set by a row of six characters, X0 X1 Y0 Y1 Z0 Z1 where,

  • X0 X1 set the type of BC on the lower and upper boundaries in x
  • Y0 Y1 set the type of BC on the lower and upper boundaries in y
  • Z0 Z1 set the type of BC on the lower and upper boundaries in z

The following options are available:

  • P periodic
  • D Dirichlet
  • N Neumann

The corresponding BC values (dummy for a periodic direction) are set in bcpsi for the volume fraction of phase 1 and in bcnor for the components of the interface normal. For consistency, the components of the interface normal should be periodic when the volume fraction boundary conditions are periodic.

Note: to conserve mass in the domain, a solid wall boundary requires a homogeneous Neumann BC for the volume fraction and a homogeneous Dirichlet BC for the wall-normal component of the interface normal. In this case, the BC for the wall-tangential components of the interface normal should be set to homogeneous Neumann.

sigma           = 1.
rho12(1:2)      = 10., 1.
mu12(1:2)       = 1.e-2, 1.e-3
ka12(1:2)       = 0., 0.
cp12(1:2)       = 0., 0.
beta12(1:2)     = 0., 0.

These lines specify the physical and transport properties of the two-phase system.

  • sigma sets the value of the surface tension coefficient at the two-phase interface.
  • rho12 sets the value of the density of each phase. (Note: the initial conditions assume rho12(1) as the densest phase)
  • mu12 sets the value of the dynamic viscosity of each phase.
  • ka12 sets the value of the thermal conductivity of each phase.
  • cp12 sets the value of the constant pressure specfic heat capacity of each phase.
  • beta12 sets the value of the thermal expansion coeffcient of each phase.
acdi_gam_factor = 1., acdi_gam_min = 0.
acdi_eps_factor = 0.51

These lines set the computational parameters specific to the conservative diffuse interface method for interface tracking. In general, these default values should be left unchanged.

  • acdi_gam_factor sets the speed of the interface relaxation, relative to the maximum flow velocity. It should always be equal to or larger than 1.
  • acdi_gam_min sets a lower threshold for the speed of the interface relaxation.
  • acdi_eps_factor sets the interface thickness relative to the maximum grid size. It should always be larger than 0.5.

about the &cudecomp namelist under input.nml

In addition to the &dns namelist in the input file, there is an optional namelist to set some runtime configurations for the cuDecomp library. Consider the following &cudecomp namelist, which corresponds to the default options in case the file is not provided:

&cudecomp
cudecomp_t_comm_backend = 0, cudecomp_is_t_enable_nccl = T, cudecomp_is_t_enable_nvshmem = T
cudecomp_h_comm_backend = 0, cudecomp_is_h_enable_nccl = T, cudecomp_is_h_enable_nvshmem = T

The first line sets the configuration for the transpose communication backend autotuning. Here cudecomp_t_comm_backend can be one of:

  • 1 -> CUDECOMP_TRANSPOSE_COMM_MPI_P2P
  • 2 -> CUDECOMP_TRANSPOSE_COMM_MPI_P2P_PL
  • 3 -> CUDECOMP_TRANSPOSE_COMM_MPI_A2A
  • 4 -> CUDECOMP_TRANSPOSE_COMM_NCCL
  • 5 -> CUDECOMP_TRANSPOSE_COMM_NCCL_PL
  • 6 -> CUDECOMP_TRANSPOSE_COMM_NVSHMEM
  • 7 -> CUDECOMP_TRANSPOSE_COMM_NVSHMEM_PL
  • any other value -> enable runtime transpose backend autotuning

The other two boolean values, enable/disable the NCCL (cudecomp_is_t_enable_nccl) and NVSHMEM (cudecomp_is_t_enable_nvshmem) options for transpose communication backend autotuning.

The second line is analogous to the first one, but for halo communication backend autotuning. Here cudecomp_h_comm_backend can be one of:

  • 1 -> CUDECOMP_HALO_COMM_MPI
  • 2 -> CUDECOMP_HALO_COMM_MPI_BLOCKING
  • 3 -> CUDECOMP_HALO_COMM_NCCL
  • 4 -> CUDECOMP_HALO_COMM_NVSHMEM
  • 5 -> CUDECOMP_HALO_COMM_NVSHMEM_BLOCKING
  • any other value -> enable runtime halo backend autotuning

The other two boolean values, enable/disable the NCCL (cudecomp_is_h_enable_nccl) and NVSHMEM (cudecomp_is_h_enable_nvshmem) options for halo communication backend autotuning.

Finally, it is worth recalling that passing dims(1:2) = [0,0] under &dns will trigger the processor grid autotuning, so there is no need to provide that option in the &cudecomp namelist.