Skip to content

Latest commit

 

History

History
253 lines (181 loc) · 12.1 KB

INFO_INPUT.md

File metadata and controls

253 lines (181 loc) · 12.1 KB
Raw

about the input file input.nml

Consider the following input file as example (corresponds to a turbulent plane channel flow). &dns defines a so-called Fortran namelist containing all the necessary physical and 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
visci = 5640.
inivel = 'poi'
is_wallturb = T
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.
is_forced(1:3) = T, F, F
velf(1:3) = 1., 0., 0.
dims(1:2) = 2, 2
\
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

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.

visci = 5640.

This line defines the inverse of the fluid viscosity, visci, meaning that the viscosity is visc = visci**(-1). Note that, for a setup defined with unit reference length and velocity scales, visci has the same value as the flow Reynolds number.

inivel = 'poi'
is_wallturb = T

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
  • 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
  • ant: three-dimensional Antuono vortex

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.

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; currently the forcing pressure gradient and time step history are reported
  • 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. Set any of these variables to 0 to skip the corresponding operation.

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).

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

  • X0 X1 set the type of BC the field variable for the lower and upper boundaries in x
  • Y0 Y1 set the type of BC the field variable for the lower and upper boundaries in y
  • Z0 Z1 set the type of BC the field variable for 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.
is_forced(1:3) = T, F, F
velf(1:3) = 1., 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.

is_forced, if true in the direction in question, forces the flow with a pressure gradient that balances the total wall shear (e.g., for a pressure-driven channel). The three boolean values correspond to three domain directions.

velf, is the target bulk velocity in the direction in question (where is_forced is true). The three values correspond to three domain directions.

dims(1:2) = 2, 2

This line set 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.

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.