Tutorial

Compile

For most systems, CaLES can be compiled from the root directory with the following commands make libs && make, which will compile the 2DECOMP&FFT/cuDecomp libraries and CaLES. make clean clears the CaLES build files, make libsclean clears the 2DECOMP/cuDecomp builds, and make allclean clears both.

The Makefile in root directory is used to compiled the code, and is expected to work out-of-the-box for most systems. The build.conf file in the root directory can be used to choose the Fortran compiler (MPI wrapper), a few pre-defined profiles depending on the nature of the run (e.g., production vs debugging), and pre-processing options:

# compiler and compiling profile
#
FCOMP=GNU           # options: GNU, NVIDIA, INTEL
FFLAGS_OPT=1        # for production runs
FFLAGS_OPT_MAX=0    # for production runs (more aggressive optimization)
FFLAGS_DEBUG=0      # for debugging
FFLAGS_DEBUG_MAX=0  # for thorough debugging
#
# defines
#
DEBUG=1                    # best = 1 (no significant performance penalty)
TIMING=1                   # best = 1
IMPDIFF=0                  #
IMPDIFF_1D=0               #
PENCIL_AXIS=1              # = 1/2/3 for X/Y/Z-aligned pencils
SINGLE_PRECISION=0         # perform the whole calculation in single precision
#
# GPU-related
#
GPU=0
USE_NVTX=0

In this file, FCOMP can be one of GNU (gfortran), INTEL (ifort), NVIDIA (nvfortran), or CRAY (ftn); the predefined profiles for compiler options can be selected by choosing one of the FFLAGS_* option; finer control of the compiler flags may be achieved by building with, e.g., make FFLAGS+=[OTHER_FLAGS], or by tweaking the profiles directly under configs/flags.mk. Similarly, the library paths (e.g., for FFTW) may need to be adapted in the Makefile (LIBS variable) or by building with make LIBS+='-L[PATH_TO_LIB] -l[NAME_OF_LIB]'. Finally, the following pre-processing options are available:

  • DEBUG : performs some basic checks for debugging purposes

  • TIMING : wall-clock time per time step is computed

  • IMPDIFF : diffusion term of the N-S equations is integrated in time with an implicit discretization (thereby improving the stability of the numerical algorithm for viscous-dominated flows)

  • IMPDIFF_1D : same as above, but with implicit diffusion only along Z; for optimal parallel performance this option should be combined with PENCIL_AXIS=3

  • PENCIL_AXIS : sets the default pencil direction, one of [1,2,3] for [X,Y,Z]-aligned pencils; X-aligned is the default and should be optimal for all cases except for Z implicit diffusion, where using Z-pencils is recommended

  • SINGLE_PRECISION : calculation will be carried out in single precision (the default precision is double)

  • GPU : enable GPU accelerated runs (requires the FCOMP=NVIDIA)

  • USE_NVTX : enable NVTX markers to tag certain code regions and assist with profiling

Typing make libs will build the 2DECOMP&FFT/cuDecomp libraries; then typing make will compile the code and create the executable cales in build/.

Note that cuDecomp needs to be dynamically linked before performing a GPU run. To do this, one should update the LD_LIBRARY_PATH environment variable as follows (from the root directory):

export LD_LIBRARY_PATH=$PWD/dependencies/cuDecomp/build/lib:$LD_LIBRARY_PATH

Finally, the choice of compiler FCOMP (see configs/flags.mk), and profile flags FFLAGS_* (see configs/flags.mk) can easily be overloaded, for instance, as: make FC=ftn FFLAGS=-O2. Linking and Include options can be changed in configs/libs.mk.

Input

Setting input.nml

Consider the following input file as an example of wall-modeled LES (WMLES) of a turbulent plane channel flow. The &dns namelist contains the necessary physical and computational parameters to set a case. The &les namelist includes parameters for the large-eddy simulation model. The &cudecomp namelist is optional and sets some runtime configurations for the cuDecomp library.

&dns
ng(1:3) = 128, 96, 64
l(1:3) = 12.8, 4.8, 2.
gtype = 6, gr = 0.
cfl = 0.95, dtmin = 1.e5
visci = 125000.
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'
cbcsgs(0:1,1:3)   = 'P','P',  'P','P',  'D','D'
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.
bcsgs(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

&les
sgstype = 'smag'
lwm(0:1,1:3) = 0,0, 0,0, 1,1
hwm = 0.1

&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

Here is a tip for vim/nvim users. Consider adding the following lines in your .vimrc file for syntax highlighting of the namelist file:

# vim
if has("autocmd")
    au BufNewFile,BufRead *.nml set filetype=fortran
    au BufNewFile,BufRead *.namelist set filetype=fortran
endif

Namelist &dns

ng(1:3) = 128, 96, 64
l(1:3) = 12.8, 4.8, 2.
gtype = 6, 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

  • 5: grid clustered towards both ends naturally

  • 6: grid clustered towards both ends suitable for WMLES of wall-bounded flows

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 = 125000.

This line defines the inverse of the fluid viscosity, visci, meaning that the viscosity is visc = visci**(-1). For a setup defined with two unit reference lengths and velocity scales, visci is half of the flow Reynolds number, as in the given example. 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.

inivel 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

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.

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'
cbcsgs(0:1,1:3)   = 'P','P',  'P','P',  'D','D'
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.
bcsgs(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 first five rows correspond to the three velocity components, pressure and eddy viscosoty, i.e. u, v, w, p and visct. The following options are available:

  • P periodic

  • D Dirichlet

  • N Neumann

The next five rows follow the same logic but specify the boundary condition values (dummy for a periodic direction). When a wall model is applied to a wall, the boundary condition for that wall should be set to a no-slip condition as given in the example.

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.

Namelist &les

sgstype = 'smag'
lwm(0:1,1:3) = 0,0, 0,0, 1,1
hwm = 0.1

These lines set the subgrid-scale (SGS) model and wall model for the large-eddy simulation.

sgstype is the type of subgrid-scale model. The following options are available:

  • smag: classical Smagorinsky model with the van Driest damping function

  • dsmag: dynamic Smagorinsky model with Lilly’s modification

lwm(0:1,1:3) sets the types of wall model for the LES. The first row corresponds to the lower wall, and the second row to the upper wall. The three columns correspond to the three domain directions. Different wall models can be applied to each wall and direction. The following options are available:

  • 0: no wall model

  • 1: logarithmic law wall model

hwm is the wall-modeled layer thickness.

Namelist &cudecomp

This 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.

Visualization

In addition to the binary files for visualization, CaLES now generates a log file that contains information about the saved data (see out2d.h90 and out3d.h90 for more details); this new approach uses that log file to generate the Xdmf visualization file.

The steps are as follows:

  1. After the simulation has run, copy the contents of utils/visualize_fields/gen_xdmf_easy/write_xdmf.py to the simulation data folder.

  2. Run the file with python write_xdmf.py.

  3. Load the generated Xdmf (*.xmf) file using paraview/visit or other visualization software.

3D fields

When running the script write_xdmf.py we get the following prompts:

# python write_xdmf.py
Name of the log file written by CaLES [log_visu_3d.out]:
Name to be appended to the grid files to prevent overwriting []:
Name of the output file [viewfld_DNS.xmf]:

  • The first value is the name of the file that logged the saved data.

  • The second is a name to append to the grid files that are generated, which should change for different log files to prevent conflicts.

  • The third is the name of the visualization file.

by pressing <kbd>enter</kbd> three times, the default values in the square brackets are assumed by the script; these correspond to the default steps required for visualizing 3D field data.

2D fields

The procedure for visualizing 2D field data that is saved by CaLES in out2d.h90 is exactly the same; it is just that the correct log file should be selected. CaLES saves by default field data in a plane of constant y=ly/2, and logs the saves to a file named log_visu_2d_slice_1.out. If more planes are saved, the user should make sure that one log file per plane is saved by CaLES (e.g. if another plane is saved, the log file written in out2d.h90 could be named log_visu_2d_slice_2.out); see out2d.h90 for more details. The corresponding steps to generate the Xdmf file would be, for instance:

# python write_xdmf.py
Name of the log file written by CaLES [log_visu_3d.out]: log_visu_2d_slice_1.out
Name to be appended to the grid files to prevent overwriting []: 2d
Name of the output file [viewfld_DNS.xmf]: viewfld_DNS_2d.xmf

Checkpoint files

A similar script also located in utils/visualize_fields/gen_xdmf_easy, named write_xdmf_restart.py, can be used to generate metadata that allows to visualize the field data contained in all saved checkpoint files:

# python write_xdmf_restart.py
Name of the pattern of the restart files to be visualized [fld?*.bin]:
Names of stored variables [VEX VEY VEZ PRE]:
Name to be appended to the grid files to prevent overwriting [_fld]:
Name of the output file [viewfld_DNS_fld.xmf]: