Compressible Navier-Stokes mini-app

This example is located in the subdirectory examples/fluids. It solves the time-dependent Navier-Stokes equations of compressible gas dynamics in a static Eulerian three-dimensional frame using unstructured high-order finite/spectral element spatial discretizations and explicit or implicit high-order time-stepping (available in PETSc). Moreover, the Navier-Stokes example has been developed using PETSc, so that the pointwise physics (defined at quadrature points) is separated from the parallelization and meshing concerns.

Running the mini-app

The Navier-Stokes mini-app is controlled via command-line options. The following options are common among all problem types:

Table 1 Common Runtime Options
Option	Description	Default value
`-ceed`	CEED resource specifier	`/cpu/self/opt/blocked`
`-test_type`	Run in test mode and specify whether solution (`solver`) or turbulent statistics (`turb_spanstats`) output should be verified	`none`
`-compare_final_state_atol`	Test absolute tolerance	`1E-11`
`-compare_final_state_filename`	Test filename
`-problem`	Problem to solve (`advection`, `advection2d`, `density_current`, `euler_vortex`, `shocktube`, `blasius`, `channel`, `gaussian_wave`, and `taylor_green`)	`density_current`
`-implicit`	Use implicit time integrator formulation
`-degree`	Polynomial degree of tensor product basis (must be >= 1)	`1`
`-q_extra`	Number of extra quadrature points	`0`
`-ts_monitor_solution`	PETSc output format, such as `cgns:output-%d.cgns` (requires PETSc `--download-cgns`)
`-ts_monitor_solution_interval`	Number of time steps between visualization output frames.	`1`
`-viewer_cgns_batch_size`	Number of frames written per CGNS file if the CGNS file name includes a format specifier (`%d`).	`20`
`-checkpoint_interval`	Number of steps between writing binary checkpoints. `0` has no output, `-1` outputs final state only	`10`
`-checkpoint_vtk`	Checkpoints include VTK (`*.vtu`) files for visualization. Consider `-ts_monitor_solution`instead.	`false`
`-viz_refine`	Use regular refinement for VTK visualization	`0`
`-output_dir`	Output directory for binary checkpoints and VTK files (if enabled).	`.`
`-output_add_stepnum2bin`	Whether to add step numbers to output binary files	`false`
`-continue`	Continue from previous solution (input is step number of previous solution)	`0`
`-continue_filename`	Path to solution binary file from which to continue from	`[output_dir]/ns-solution.bin`
`-continue_time_filename`	Path to time stamp binary file (only for legacy checkpoints)	`[output_dir]/ns-time.bin`
`-bc_wall`	Use wall boundary conditions on this list of faces
`-wall_comps`	An array of constrained component numbers for wall BCs
`-bc_slip_x`	Use slip boundary conditions, for the x component, on this list of faces
`-bc_slip_y`	Use slip boundary conditions, for the y component, on this list of faces
`-bc_slip_z`	Use slip boundary conditions, for the z component, on this list of faces
`-bc_inflow`	Use inflow boundary conditions on this list of faces
`-bc_outflow`	Use outflow boundary conditions on this list of faces
`-bc_freestream`	Use freestream boundary conditions on this list of faces
`-ts_monitor_turbulence_spanstats_collect_interval`	Number of timesteps between statistics collection	`1`
`-ts_monitor_turbulence_spanstats_viewer`	Sets the PetscViewer for the statistics file writing, such as `cgns:output-%d.cgns` (requires PETSc `--download-cgns`). Also turns the statistics collection on.
`-ts_monitor_turbulence_spanstats_viewer_interval`	Number of timesteps between statistics file writing (`-1` means only at end of run)	`-1`
`-ts_monitor_turbulence_spanstats_viewer_cgns_batch_size`	Number of frames written per CGNS file if the CGNS file name includes a format specifier (`%d`).	`20`
`-ts_monitor_wall_force`	Viewer for the force on each no-slip wall, e.g., `ascii:force.csv:ascii_csv` to write a CSV file.
`-mesh_transform`	Transform the mesh, usually for an initial box mesh.	`none`
`-snes_view`	View PETSc `SNES` nonlinear solver configuration
`-log_view`	View PETSc performance log
`-help`	View comprehensive information about run-time options

For the case of a square/cubic mesh, the list of face indices to be used with -bc_wall, bc_inflow, bc_outflow, bc_freestream and/or -bc_slip_x, -bc_slip_y, and -bc_slip_z are:

Table 2 2D Face ID Labels
PETSc Face Name	Cartesian direction	Face ID
faceMarkerBottom	-z	1
faceMarkerRight	+x	2
faceMarkerTop	+z	3
faceMarkerLeft	-x	4

Table 3 3D Face ID Labels
PETSc Face Name	Cartesian direction	Face ID
faceMarkerBottom	-z	1
faceMarkerTop	+z	2
faceMarkerFront	-y	3
faceMarkerBack	+y	4
faceMarkerRight	+x	5
faceMarkerLeft	-x	6

Boundary conditions

Boundary conditions for compressible viscous flows are notoriously tricky. Here we offer some recommendations.

Inflow

If in a region where the flow velocity is known (e.g., away from viscous walls), use bc_freestream, which solves a Riemann problem and can handle inflow and outflow (simultaneously and dynamically). It is stable and the least reflective boundary condition for acoustics.

If near a viscous wall, you may want a specified inflow profile. Use bc_inflow and see Blasius boundary layer and discussion of synthetic turbulence generation for ways to analytically generate developed inflow profiles. These conditions may be either weak or strong, with the latter specifying velocity and temperature as essential boundary conditions and evaluating a boundary integral for the mass flux. The strong approach gives sharper resolution of velocity structures. We have described the primitive variable formulation here; the conservative variants are similar, but not equivalent.

Outflow

If you know the complete exterior state, bc_freestream is the least reflective boundary condition, but is disruptive to viscous flow structures. If thermal anomalies must exit the domain, the Riemann solver must resolve the contact wave to avoid reflections. The default Riemann solver, HLLC, is sufficient in this regard while the simpler HLL converts thermal structures exiting the domain into grid-scale reflecting acoustics.

If acoustic reflections are not a concern and/or the flow is impacted by walls or interior structures that you wish to resolve to near the boundary, choose bc_outflow. This condition (with default outflow_type: riemann) is stable for both inflow and outflow, so can be used in areas that have recirculation and lateral boundaries in which the flow fluctuates.

The simpler bc_outflow variant, outflow_type: pressure, requires that the flow be a strict outflow (or the problem becomes ill-posed and the solver will diverge). In our experience, riemann is slightly less reflective but produces similar flows in cases of strict outflow. The pressure variant is retained to facilitate comparison with other codes, such as PHASTA-C, but we recommend riemann for general use.

Periodicity

PETSc provides two ways to specify periodicity:

Topological periodicity, in which the donor and receiver dofs are the same, obtained using:

dm_plex:
  shape: box
  box_faces: 10,12,4
  box_bd: none,none,periodic

The coordinates for such cases are stored as a new field with special cell-based indexing to enable wrapping through the boundary. This choice of coordinates prevents evaluating boundary integrals that cross the periodicity, such as for the outflow Riemann problem in the presence of spanwise periodicity.

Isoperiodicity, in which the donor and receiver dofs are distinct in local vectors. This is obtained using zbox, as in:

dm_plex:
  shape: zbox
  box_faces: 10,12,4
  box_bd: none,none,periodic

Isoperiodicity enables standard boundary integrals, and is recommended for general use. At the time of this writing, it only supports one direction of periodicity. The zbox method uses Z-ordering to construct the mesh in parallel and provide an adequate initial partition, which makes it higher performance and avoids needing a partitioning package.

Advection

For testing purposes, there is a reduced mode for pure advection, which holds density \(\rho\) and momentum density \(\rho \bm u\) constant while advecting “total energy density” \(E\). These are available in 2D and 3D.

2D advection

For the 2D advection problem, the following additional command-line options are available:

Table 4 Advection2D Runtime Options
Option	Description	Default value	Unit
`-rc`	Characteristic radius of thermal bubble	`1000`	`m`
`-units_meter`	1 meter in scaled length units	`1E-2`
`-units_second`	1 second in scaled time units	`1E-2`
`-units_kilogram`	1 kilogram in scaled mass units	`1E-6`
`-strong_form`	Strong (1) or weak/integrated by parts (0) residual	`0`
`-stab`	Stabilization method (`none`, `su`, or `supg`)	`none`
`-CtauS`	Scale coefficient for stabilization tau (nondimensional)	`0`
`-wind_type`	Wind type in Advection (`rotation` or `translation`)	`rotation`
`-wind_translation`	Constant wind vector when `-wind_type translation`	`1,0,0`
`-E_wind`	Total energy of inflow wind when `-wind_type translation`	`1E6`	`J`

An example of the rotation mode can be run with:

./navierstokes -problem advection2d -dm_plex_box_faces 20,20 -dm_plex_box_lower 0,0 -dm_plex_box_upper 1000,1000 -bc_wall 1,2,3,4 -wall_comps 4 -wind_type rotation -implicit -stab supg

and the translation mode with:

./navierstokes -problem advection2d -dm_plex_box_faces 20,20 -dm_plex_box_lower 0,0 -dm_plex_box_upper 1000,1000 -units_meter 1e-4 -wind_type translation -wind_translation 1,-.5 -bc_inflow 1,2,3,4

Note the lengths in -dm_plex_box_upper are given in meters, and will be nondimensionalized according to -units_meter.

3D advection

For the 3D advection problem, the following additional command-line options are available:

Table 5 Advection3D Runtime Options
Option	Description	Default value	Unit
`-rc`	Characteristic radius of thermal bubble	`1000`	`m`
`-units_meter`	1 meter in scaled length units	`1E-2`
`-units_second`	1 second in scaled time units	`1E-2`
`-units_kilogram`	1 kilogram in scaled mass units	`1E-6`
`-strong_form`	Strong (1) or weak/integrated by parts (0) residual	`0`
`-stab`	Stabilization method (`none`, `su`, or `supg`)	`none`
`-CtauS`	Scale coefficient for stabilization tau (nondimensional)	`0`
`-wind_type`	Wind type in Advection (`rotation` or `translation`)	`rotation`
`-wind_translation`	Constant wind vector when `-wind_type translation`	`1,0,0`
`-E_wind`	Total energy of inflow wind when `-wind_type translation`	`1E6`	`J`
`-bubble_type`	`sphere` (3D) or `cylinder` (2D)	`sphere`
`-bubble_continuity`	`smooth`, `back_sharp`, or `thick`	`smooth`

An example of the rotation mode can be run with:

./navierstokes -problem advection -dm_plex_box_faces 10,10,10 -dm_plex_dim 3 -dm_plex_box_lower 0,0,0 -dm_plex_box_upper 8000,8000,8000 -bc_wall 1,2,3,4,5,6 -wall_comps 4 -wind_type rotation -implicit -stab su

and the translation mode with:

./navierstokes -problem advection -dm_plex_box_faces 10,10,10 -dm_plex_dim 3 -dm_plex_box_lower 0,0,0 -dm_plex_box_upper 8000,8000,8000 -wind_type translation -wind_translation .5,-1,0 -bc_inflow 1,2,3,4,5,6

Inviscid Ideal Gas

Isentropic Euler vortex

For the Isentropic Vortex problem, the following additional command-line options are available:

Table 6 Isentropic Vortex Runtime Options
Option	Description	Default value	Unit
`-center`	Location of vortex center	`(lx,ly,lz)/2`	`(m,m,m)`
`-units_meter`	1 meter in scaled length units	`1E-2`
`-units_second`	1 second in scaled time units	`1E-2`
`-mean_velocity`	Background velocity vector	`(1,1,0)`
`-vortex_strength`	Strength of vortex < 10	`5`
`-c_tau`	Stabilization constant	`0.5`

This problem can be run with:

./navierstokes -problem euler_vortex -dm_plex_box_faces 20,20,1 -dm_plex_box_lower 0,0,0 -dm_plex_box_upper 1000,1000,50 -dm_plex_dim 3 -bc_inflow 4,6 -bc_outflow 3,5 -bc_slip_z 1,2 -mean_velocity .5,-.8,0.

Sod shock tube

For the Shock Tube problem, the following additional command-line options are available:

Table 7 Shock Tube Runtime Options
Option	Description	Default value
`-units_meter`	1 meter in scaled length units	`1E-2`
`-units_second`	1 second in scaled time units	`1E-2`
`-yzb`	Use YZB discontinuity capturing	`none`
`-stab`	Stabilization method (`none`, `su`, or `supg`)	`none`

This problem can be run with:

./navierstokes -problem shocktube -yzb -stab su -bc_slip_z 3,4 -bc_slip_y 1,2 -bc_wall 5,6 -dm_plex_dim 3 -dm_plex_box_lower 0,0,0 -dm_plex_box_upper 1000,100,100 -dm_plex_box_faces 200,1,1 -units_second 0.1

Newtonian viscosity, Ideal Gas

For the Density Current, Channel, and Blasius problems, the following common command-line options are available:

Table 8 Newtonian Ideal Gas problems Runtime Options
Option	Description	Default value	Unit
`-units_meter`	1 meter in scaled length units	`1`
`-units_second`	1 second in scaled time units	`1`
`-units_kilogram`	1 kilogram in scaled mass units	`1`
`-units_Kelvin`	1 Kelvin in scaled temperature units	`1`
`-stab`	Stabilization method (`none`, `su`, or `supg`)	`none`
`-c_tau`	Stabilization constant, \(c_\tau\)	`0.5`
`-Ctau_t`	Stabilization time constant, \(C_t\)	`1.0`
`-Ctau_v`	Stabilization viscous constant, \(C_v\)	`36, 60, 128 for degree = 1, 2, 3`
`-Ctau_C`	Stabilization continuity constant, \(C_c\)	`1.0`
`-Ctau_M`	Stabilization momentum constant, \(C_m\)	`1.0`
`-Ctau_E`	Stabilization energy constant, \(C_E\)	`1.0`
`-cv`	Heat capacity at constant volume	`717`	`J/(kg K)`
`-cp`	Heat capacity at constant pressure	`1004`	`J/(kg K)`
`-gravity`	Gravitational acceleration vector	`0,0,0`	`m/s^2`
`-lambda`	Stokes hypothesis second viscosity coefficient	`-2/3`
`-mu`	Shear dynamic viscosity coefficient	`1.8e-5`	`Pa s`
`-k`	Thermal conductivity	`0.02638`	`W/(m K)`
`-newtonian_unit_tests`	Developer option to test properties	`false`	boolean
`-state_var`	State variables to solve solution with. `conservative` (\(\rho, \rho \bm{u}, \rho e\)) or `primitive` (\(P, \bm{u}, T\))	`conservative`	string
`-idl_decay_time`	Characteristic timescale of the pressure deviance decay. The timestep is good starting point	`-1` (disabled)	`s`
`-idl_start`	Start of IDL in the x direction	`0`	`m`
`-idl_length`	Length of IDL in the positive x direction	`0`	`m`
`-sgs_model_type`	Type of subgrid stress model to use. Currently only `data_driven` is available	`none`	string
`-sgs_model_dd_leakyrelu_alpha`	Slope parameter for Leaky ReLU activation function. `0` corresponds to normal ReLU	0
`-sgs_model_dd_parameter_dir`	Path to directory with data-driven model parameters (weights, biases, etc.)	`./dd_sgs_parameters`	string
`-diff_filter_monitor`	Enable differential filter TSMonitor	`false`	boolean
`-diff_filter_grid_based_width`	Use filter width based on the grid size	`false`	boolean
`-diff_filter_width_scaling`	Anisotropic scaling for filter width in wall-aligned coordinates (snz)	`1,1,1`	`m`
`-diff_filter_kernel_scaling`	Scaling to make differential kernel size equivalent to other filter kernels	`0.1`	`m^2`
`-diff_filter_wall_damping_function`	Damping function to use at the wall for anisotropic filtering (`none`, `van_driest`)	`none`	string
`-diff_filter_wall_damping_constant`	Constant for the wall-damping function. \(A^+\) for `van_driest` damping function.	25
`-diff_filter_friction_length`	Friction length associated with the flow, \(\delta_\nu\). Used in wall-damping functions	0	`m`
`-sgs_train_enable`	Whether to enable in situ training of data-driven SGS model. Require building with SmartRedis.	`false`	boolean
`-sgs_train_write_data_interval`	Number of timesteps between writing training data into SmartRedis database	`1`
`-sgs_train_overwrite_data`	Whether new training data should overwrite old data on database	`true`	boolean
`-smartsim_collocated_num_ranks`	Number of MPI ranks associated with each collocated database (i.e. ranks per node)	`1`

Gaussian Wave

The Gaussian wave problem has the following command-line options in addition to the Newtonian Ideal Gas options:

Table 9 Gaussian Wave Runtime Options
Option	Description	Default value	Unit
`-freestream_riemann`	Riemann solver for boundaries (HLL or HLLC)	`hllc`
`-freestream_velocity`	Freestream velocity vector	`0,0,0`	`m/s`
`-freestream_temperature`	Freestream temperature	`288`	`K`
`-freestream_pressure`	Freestream pressure	`1.01e5`	`Pa`
`-epicenter`	Coordinates of center of perturbation	`0,0,0`	`m`
`-amplitude`	Amplitude of the perturbation	`0.1`
`-width`	Width parameter of the perturbation	`0.002`	`m`

This problem can be run with the gaussianwave.yaml file via:

./navierstokes -options_file gaussianwave.yaml

problem: gaussian_wave
mu: 0 # Effectively solving Euler momentum equations

dm_plex_box_faces: 40,40,1
dm_plex_box_upper: 1,1,0.025
dm_plex_box_lower: 0,0,0
dm_plex_dim: 3
bc_freestream: 4,6,3,5
bc_slip_z: 1,2

reference:
  temperature: 0.25
  pressure: 71.75
freestream:
  # riemann: hll # causes thermal bubble to reflect acoustic waves from boundary
  velocity: 2,2,0

epicenter: 0.33,0.75,0
amplitude: 2
width: 0.05

ts:
  adapt_type: none
  max_steps: 100
  dt: 2e-3
  type: alpha
  alpha_radius: 0.5
  #monitor_solution: cgns:nwave.cgns
  #monitor_solution_interval: 10

implicit: true
stab: supg
state_var: primitive

snes_rtol: 1e-4
ksp_rtol: 1e-2
snes_lag_jacobian: 20
snes_lag_jacobian_persists:

## Demonstrate acoustic wave dissipation using an internal damping layer
# idl:
#   decay_time: 2e-3
#   start: 0
#   length: .25

Vortex Shedding - Flow past Cylinder

The vortex shedding, flow past cylinder problem has the following command-line options in addition to the Newtonian Ideal Gas options:

Table 10 Vortex Shedding Runtime Options
Option	Description	Default value	Unit
`-freestream_velocity`	Freestream velocity vector	`0,0,0`	`m/s`
`-freestream_temperature`	Freestream temperature	`288`	`K`
`-freestream_pressure`	Freestream pressure	`1.01e5`	`Pa`

The initial condition is taken from -reference_temperature and -reference_pressure. To run this problem, first generate a mesh:

$ make -C examples/fluids/meshes

Then run by building the executable and running:

$ make build/fluids-navierstokes
$ mpiexec -n 6 build/fluids-navierstokes -options_file examples/fluids/vortexshedding.yaml -{ts,snes}_monitor_

The vortex shedding period is roughly 5.6 and this problem runs until time 100 (2000 time steps). The above run writes a file named force.csv (see ts_monitor_wall_force in vortexshedding.yaml), which can be postprocessed by running to create a figure showing lift and drag coefficients over time.

$ python examples/fluids/postprocess/vortexshedding.py

problem: newtonian

# Time Stepping Settings
implicit: true
stab: supg

checkpoint_interval: 10

ts:
  adapt_type: 'none'
  type: alpha
  dt: .05
  max_time: 100
  alpha_radius: 0.5
  monitor_solution: cgns:vortexshedding-q3-g1-n08.cgns
  monitor_solution_interval: 5
  monitor_wall_force: ascii:force.csv:ascii_csv

# Reference state is used for the initial condition, zero velocity by default.

# This choice of pressure and temperature have a density of 1 and acoustic speed
# of 100. With velocity 1, this flow is Mach 0.01.
reference:
  pressure: 7143
  temperature: 24.92

# If the the outflow is placed close to the cylinder, this will recirculate cold
# fluid, demonstrating how the outflow BC is stable despite recirculation.
outflow:
  temperature: 20

# Freestream inherits reference state as default
freestream:
  velocity: 1,0,0
# Small gravity vector to break symmetry so shedding can start
g: 0,-.01,0

# viscosity corresponds to Reynolds number 100
mu: 0.01
k: 14.34 # thermal conductivity, Pr = 0.71 typical of air

## DM Settings:
degree: 3
dm_plex_filename: examples/fluids/meshes/cylinder-q1-n08.msh

# Boundary Settings
bc_slip_z: 6
bc_wall: 5
bc_freestream: 1
bc_outflow: 2
bc_slip_y: 3,4
wall_comps: 1,2,3

# Primitive variables are preferred at low Mach number
state_var: primitive

dm_view:
ts_monitor:
snes_lag_jacobian: 20
snes_lag_jacobian_persists:

#pmat_pbdiagonal:
#ksp_type: bcgsl
#pc_type: vpbjacobi
amat_type: shell

Density current

The Density Current problem has the following command-line options in addition to the Newtonian Ideal Gas options:

Table 11 Density Current Runtime Options
Option	Description	Default value	Unit
`-center`	Location of bubble center	`(lx,ly,lz)/2`	`(m,m,m)`
`-dc_axis`	Axis of density current cylindrical anomaly, or `(0,0,0)` for spherically symmetric	`(0,0,0)`
`-rc`	Characteristic radius of thermal bubble	`1000`	`m`
`-theta0`	Reference potential temperature	`300`	`K`
`-thetaC`	Perturbation of potential temperature	`-15`	`K`
`-P0`	Atmospheric pressure	`1E5`	`Pa`
`-N`	Brunt-Vaisala frequency	`0.01`	`1/s`

This problem can be run with:

./navierstokes -problem density_current -dm_plex_box_faces 16,1,8 -degree 1 -dm_plex_box_lower 0,0,0 -dm_plex_box_upper 2000,125,1000 -dm_plex_dim 3 -rc 400. -bc_wall 1,2,5,6 -wall_comps 1,2,3 -bc_slip_y 3,4 -mu 75

Channel flow

The Channel problem has the following command-line options in addition to the Newtonian Ideal Gas options:

Table 12 Channel Runtime Options
Option	Description	Default value	Unit
`-umax`	Maximum/centerline velocity of the flow	`10`	`m/s`
`-theta0`	Reference potential temperature	`300`	`K`
`-P0`	Atmospheric pressure	`1E5`	`Pa`
`-body_force_scale`	Multiplier for body force (`-1` for flow reversal)	1

This problem can be run with the channel.yaml file via:

./navierstokes -options_file channel.yaml

problem: 'channel'
mu: .01

umax: 40
implicit: true
ts:
  type: 'beuler'
  adapt_type: 'none'
  dt: 5e-6

q_extra: 2

dm_plex_box_lower: 0,0,0
dm_plex_box_upper: .01,.01,.001
dm_plex_dim: 3
degree: 1
dm_plex_box_faces: 10,10,1
bc_slip_z: 1,2
bc_wall: 3,4
wall_comps: 1,2,3
dm_plex_box_bd: 'periodic,none,none'

Blasius boundary layer

The Blasius problem has the following command-line options in addition to the Newtonian Ideal Gas options:

Table 13 Blasius Runtime Options
Option	Description	Default value	Unit
`-velocity_infinity`	Freestream velocity	`40`	`m/s`
`-temperature_infinity`	Freestream temperature	`288`	`K`
`-temperature_wall`	Wall temperature	`288`	`K`
`-delta0`	Boundary layer height at the inflow	`4.2e-3`	`m`
`-P0`	Atmospheric pressure	`1.01E5`	`Pa`
`-platemesh_modify_mesh`	Whether to modify the mesh using the given options below.	`false`
`-platemesh_refine_height`	Height at which `-platemesh_Ndelta` number of elements should refined into	`5.9E-4`	`m`
`-platemesh_Ndelta`	Number of elements to keep below `-platemesh_refine_height`	`45`
`-platemesh_growth`	Growth rate of the elements in the refinement region	`1.08`
`-platemesh_top_angle`	Downward angle of the top face of the domain. This face serves as an outlet.	`5`	`degrees`
`-platemesh_y_node_locs_path`	Path to file with y node locations. If empty, will use mesh warping instead.	`""`
`-stg_use`	Whether to use STG for the inflow conditions	`false`
`-n_chebyshev`	Number of Chebyshev terms	`20`
`-chebyshev_`	Prefix for Chebyshev snes solve

This problem can be run with the blasius.yaml file via:

./navierstokes -options_file blasius.yaml

problem: 'blasius'

implicit: true
ts:
  adapt_type: 'none'
  type: 'beuler'
  dt: 2e-6
  max_time: 1.0e-3
  #monitor_solution: cgns:blasius-%d.cgns
  #monitor_solution_interval: 10
checkpoint_interval: 10

## Linear Settings:
degree: 1
dm_plex_box_faces: 40,60,1
mesh_transform: platemesh
platemesh_nDelta: 45

# # Quadratic Settings:
# degree: 2
# dm_plex_box_faces: 20,30,1
# platemesh:
#   modify_mesh: true
#   nDelta: 22
#   growth: 1.1664 # 1.08^2

stab: 'supg'

dm_plex_box_lower: 0,0,0
dm_plex_box_upper: 4.2e-3,4.2e-3,5.e-5
dm_plex_dim: 3
# Faces labeled 1=z- 2=z+ 3=y- 4=y+ 5=x+ 6=x-
bc_slip_z: 1,2
bc_wall: 3
wall_comps: 1,2,3
bc_inflow: 6
bc_outflow: 5,4
gravity: 0,0,0

stg:
  use: false
  inflow_path: "./STGInflow_blasius.dat"
  mean_only: true

# ts_monitor_turbulence_spanstats:
#   collect_interval: 1
#   viewer_interval: 5
#   viewer: cgns:stats-%d.cgns
#   viewer_cgns_batch_size: 1

STG Inflow for Flat Plate

Using the STG Inflow for the blasius problem adds the following command-line options:

Table 14 Blasius Runtime Options
Option	Description	Default value	Unit
`-stg_inflow_path`	Path to the STGInflow file	`./STGInflow.dat`
`-stg_rand_path`	Path to the STGRand file	`./STGRand.dat`
`-stg_alpha`	Growth rate of the wavemodes	`1.01`
`-stg_u0`	Convective velocity, \(U_0\)	`0.0`	`m/s`
`-stg_mean_only`	Only impose the mean velocity (no fluctutations)	`false`
`-stg_strong`	Strongly enforce the STG inflow boundary condition	`false`
`-stg_fluctuating_IC`	“Extrude” the fluctuations through the domain as an initial condition	`false`

This problem can be run with the blasius.yaml file via:

./navierstokes -options_file blasius.yaml -stg_use true

Note the added -stg_use true flag This overrides the stg: use: false setting in the blasius.yaml file, enabling the use of the STG inflow.

The Navier-Stokes equations

The mathematical formulation (from [SHJ91]) is given in what follows. The compressible Navier-Stokes equations in conservative form are

(15)\[ \begin{aligned} \frac{\partial \rho}{\partial t} + \nabla \cdot \bm{U} &= 0 \\ \frac{\partial \bm{U}}{\partial t} + \nabla \cdot \left( \frac{\bm{U} \otimes \bm{U}}{\rho} + P \bm{I}_3 -\bm\sigma \right) - \rho \bm{b} &= 0 \\ \frac{\partial E}{\partial t} + \nabla \cdot \left( \frac{(E + P)\bm{U}}{\rho} -\bm{u} \cdot \bm{\sigma} - k \nabla T \right) - \rho \bm{b} \cdot \bm{u} &= 0 \, , \\ \end{aligned} \]

where \(\bm{\sigma} = \mu(\nabla \bm{u} + (\nabla \bm{u})^T + \lambda (\nabla \cdot \bm{u})\bm{I}_3)\) is the Cauchy (symmetric) stress tensor, with \(\mu\) the dynamic viscosity coefficient, and \(\lambda = - 2/3\) the Stokes hypothesis constant. In equations (15), \(\rho\) represents the volume mass density, \(U\) the momentum density (defined as \(\bm{U}=\rho \bm{u}\), where \(\bm{u}\) is the vector velocity field), \(E\) the total energy density (defined as \(E = \rho e\), where \(e\) is the total energy including thermal and kinetic but not potential energy), \(\bm{I}_3\) represents the \(3 \times 3\) identity matrix, \(\bm{b}\) is a body force vector (e.g., gravity vector \(\bm{g}\)), \(k\) the thermal conductivity constant, \(T\) represents the temperature, and \(P\) the pressure, given by the following equation of state

(16)\[ P = \left( {c_p}/{c_v} -1\right) \left( E - {\bm{U}\cdot\bm{U}}/{(2 \rho)} \right) \, , \]

where \(c_p\) is the specific heat at constant pressure and \(c_v\) is the specific heat at constant volume (that define \(\gamma = c_p / c_v\), the specific heat ratio).

The system (15) can be rewritten in vector form

(17)\[ \frac{\partial \bm{q}}{\partial t} + \nabla \cdot \bm{F}(\bm{q}) -S(\bm{q}) = 0 \, , \]

for the state variables 5-dimensional vector

\[ \bm{q} = \begin{pmatrix} \rho \\ \bm{U} \equiv \rho \bm{ u }\\ E \equiv \rho e \end{pmatrix} \begin{array}{l} \leftarrow\textrm{ volume mass density}\\ \leftarrow\textrm{ momentum density}\\ \leftarrow\textrm{ energy density} \end{array} \]

where the flux and the source terms, respectively, are given by

(18)\[ \begin{aligned} \bm{F}(\bm{q}) &= \underbrace{\begin{pmatrix} \bm{U}\\ {(\bm{U} \otimes \bm{U})}/{\rho} + P \bm{I}_3 \\ {(E + P)\bm{U}}/{\rho} \end{pmatrix}}_{\bm F_{\text{adv}}} + \underbrace{\begin{pmatrix} 0 \\ - \bm{\sigma} \\ - \bm{u} \cdot \bm{\sigma} - k \nabla T \end{pmatrix}}_{\bm F_{\text{diff}}},\\ S(\bm{q}) &= \begin{pmatrix} 0\\ \rho \bm{b}\\ \rho \bm{b}\cdot \bm{u} \end{pmatrix}. \end{aligned} \]

Finite Element Formulation (Spatial Discretization)

Let the discrete solution be

\[ \bm{q}_N (\bm{x},t)^{(e)} = \sum_{k=1}^{P}\psi_k (\bm{x})\bm{q}_k^{(e)} \]

with \(P=p+1\) the number of nodes in the element \(e\). We use tensor-product bases \(\psi_{kji} = h_i(X_0)h_j(X_1)h_k(X_2)\).

To obtain a finite element discretization, we first multiply the strong form (17) by a test function \(\bm v \in H^1(\Omega)\) and integrate,

\[ \int_{\Omega} \bm v \cdot \left(\frac{\partial \bm{q}_N}{\partial t} + \nabla \cdot \bm{F}(\bm{q}_N) - \bm{S}(\bm{q}_N) \right) \,dV = 0 \, , \; \forall \bm v \in \mathcal{V}_p\,, \]

with \(\mathcal{V}_p = \{ \bm v(\bm x) \in H^{1}(\Omega_e) \,|\, \bm v(\bm x_e(\bm X)) \in P_p(\bm{I}), e=1,\ldots,N_e \}\) a mapped space of polynomials containing at least polynomials of degree \(p\) (with or without the higher mixed terms that appear in tensor product spaces).

Integrating by parts on the divergence term, we arrive at the weak form,

(19)\[ \begin{aligned} \int_{\Omega} \bm v \cdot \left( \frac{\partial \bm{q}_N}{\partial t} - \bm{S}(\bm{q}_N) \right) \,dV - \int_{\Omega} \nabla \bm v \!:\! \bm{F}(\bm{q}_N)\,dV & \\ + \int_{\partial \Omega} \bm v \cdot \bm{F}(\bm q_N) \cdot \widehat{\bm{n}} \,dS &= 0 \, , \; \forall \bm v \in \mathcal{V}_p \,, \end{aligned} \]

where \(\bm{F}(\bm q_N) \cdot \widehat{\bm{n}}\) is typically replaced with a boundary condition.

Note

The notation \(\nabla \bm v \!:\! \bm F\) represents contraction over both fields and spatial dimensions while a single dot represents contraction in just one, which should be clear from context, e.g., \(\bm v \cdot \bm S\) contracts over fields while \(\bm F \cdot \widehat{\bm n}\) contracts over spatial dimensions.

Time Discretization

For the time discretization, we use two types of time stepping schemes through PETSc.

Explicit time-stepping method

The following explicit formulation is solved with the adaptive Runge-Kutta-Fehlberg (RKF4-5) method by default (any explicit time-stepping scheme available in PETSc can be chosen at runtime)

\[ \bm{q}_N^{n+1} = \bm{q}_N^n + \Delta t \sum_{i=1}^{s} b_i k_i \, , \]

where

\[ \begin{aligned} k_1 &= f(t^n, \bm{q}_N^n)\\ k_2 &= f(t^n + c_2 \Delta t, \bm{q}_N^n + \Delta t (a_{21} k_1))\\ k_3 &= f(t^n + c_3 \Delta t, \bm{q}_N^n + \Delta t (a_{31} k_1 + a_{32} k_2))\\ \vdots&\\ k_i &= f\left(t^n + c_i \Delta t, \bm{q}_N^n + \Delta t \sum_{j=1}^s a_{ij} k_j \right)\\ \end{aligned} \]

and with

\[ f(t^n, \bm{q}_N^n) = - [\nabla \cdot \bm{F}(\bm{q}_N)]^n + [S(\bm{q}_N)]^n \, . \]

Implicit time-stepping method

This time stepping method which can be selected using the option -implicit is solved with Backward Differentiation Formula (BDF) method by default (similarly, any implicit time-stepping scheme available in PETSc can be chosen at runtime). The implicit formulation solves nonlinear systems for \(\bm q_N\):

(20)\[ \bm f(\bm q_N) \equiv \bm g(t^{n+1}, \bm{q}_N, \bm{\dot{q}}_N) = 0 \, , \]

where the time derivative \(\bm{\dot q}_N\) is defined by

\[ \bm{\dot{q}}_N(\bm q_N) = \alpha \bm q_N + \bm z_N \]

in terms of \(\bm z_N\) from prior state and \(\alpha > 0\), both of which depend on the specific time integration scheme (backward difference formulas, generalized alpha, implicit Runge-Kutta, etc.). Each nonlinear system (20) will correspond to a weak form, as explained below. In determining how difficult a given problem is to solve, we consider the Jacobian of (20),

\[ \frac{\partial \bm f}{\partial \bm q_N} = \frac{\partial \bm g}{\partial \bm q_N} + \alpha \frac{\partial \bm g}{\partial \bm{\dot q}_N}. \]

The scalar “shift” \(\alpha\) scales inversely with the time step \(\Delta t\), so small time steps result in the Jacobian being dominated by the second term, which is a sort of “mass matrix”, and typically well-conditioned independent of grid resolution with a simple preconditioner (such as Jacobi). In contrast, the first term dominates for large time steps, with a condition number that grows with the diameter of the domain and polynomial degree of the approximation space. Both terms are significant for time-accurate simulation and the setup costs of strong preconditioners must be balanced with the convergence rate of Krylov methods using weak preconditioners.

More details of PETSc’s time stepping solvers can be found in the TS User Guide.

Stabilization

We solve (19) using a Galerkin discretization (default) or a stabilized method, as is necessary for most real-world flows.

Galerkin methods produce oscillations for transport-dominated problems (any time the cell Péclet number is larger than 1), and those tend to blow up for nonlinear problems such as the Euler equations and (low-viscosity/poorly resolved) Navier-Stokes, in which case stabilization is necessary. Our formulation follows [HST10], which offers a comprehensive review of stabilization and shock-capturing methods for continuous finite element discretization of compressible flows.

SUPG (streamline-upwind/Petrov-Galerkin)

In this method, the weighted residual of the strong form (17) is added to the Galerkin formulation (19). The weak form for this method is given as

(21)\[ \begin{aligned} \int_{\Omega} \bm v \cdot \left( \frac{\partial \bm{q}_N}{\partial t} - \bm{S}(\bm{q}_N) \right) \,dV - \int_{\Omega} \nabla \bm v \!:\! \bm{F}(\bm{q}_N)\,dV & \\ + \int_{\partial \Omega} \bm v \cdot \bm{F}(\bm{q}_N) \cdot \widehat{\bm{n}} \,dS & \\ + \int_{\Omega} \nabla\bm v \tcolon\left(\frac{\partial \bm F_{\text{adv}}}{\partial \bm q}\right) \bm\tau \left( \frac{\partial \bm{q}_N}{\partial t} \, + \, \nabla \cdot \bm{F} \, (\bm{q}_N) - \bm{S}(\bm{q}_N) \right) \,dV &= 0 \, , \; \forall \bm v \in \mathcal{V}_p \end{aligned} \]

This stabilization technique can be selected using the option -stab supg.
SU (streamline-upwind)

This method is a simplified version of SUPG (21) which is developed for debugging/comparison purposes. The weak form for this method is

(22)\[ \begin{aligned} \int_{\Omega} \bm v \cdot \left( \frac{\partial \bm{q}_N}{\partial t} - \bm{S}(\bm{q}_N) \right) \,dV - \int_{\Omega} \nabla \bm v \!:\! \bm{F}(\bm{q}_N)\,dV & \\ + \int_{\partial \Omega} \bm v \cdot \bm{F}(\bm{q}_N) \cdot \widehat{\bm{n}} \,dS & \\ + \int_{\Omega} \nabla\bm v \tcolon\left(\frac{\partial \bm F_{\text{adv}}}{\partial \bm q}\right) \bm\tau \nabla \cdot \bm{F} \, (\bm{q}_N) \,dV & = 0 \, , \; \forall \bm v \in \mathcal{V}_p \end{aligned} \]

This stabilization technique can be selected using the option -stab su.

In both (22) and (21), \(\bm\tau \in \mathbb R^{5\times 5}\) (field indices) is an intrinsic time scale matrix. The SUPG technique and the operator \(\frac{\partial \bm F_{\text{adv}}}{\partial \bm q}\) (rather than its transpose) can be explained via an ansatz for subgrid state fluctuations \(\tilde{\bm q} = -\bm\tau \bm r\) where \(\bm r\) is a strong form residual. The forward variational form can be readily expressed by differentiating \(\bm F_{\text{adv}}\) of (18)

\[ \begin{aligned} \diff\bm F_{\text{adv}}(\diff\bm q; \bm q) &= \frac{\partial \bm F_{\text{adv}}}{\partial \bm q} \diff\bm q \\ &= \begin{pmatrix} \diff\bm U \\ (\diff\bm U \otimes \bm U + \bm U \otimes \diff\bm U)/\rho - (\bm U \otimes \bm U)/\rho^2 \diff\rho + \diff P \bm I_3 \\ (E + P)\diff\bm U/\rho + (\diff E + \diff P)\bm U/\rho - (E + P) \bm U/\rho^2 \diff\rho \end{pmatrix}, \end{aligned} \]

where \(\diff P\) is defined by differentiating (16).

Currently, this demo provides three types of problems/physical models that can be selected at run time via the option -problem. Advection, the problem of the transport of energy in a uniform vector velocity field, Isentropic Vortex, the exact solution to the Euler equations, and the so called Gaussian Wave problem.

Subgrid Stress Modeling

When a fluid simulation is under-resolved (the smallest length scale resolved by the grid is much larger than the smallest physical scale, the Kolmogorov length scale), this is mathematically interpreted as filtering the Navier-Stokes equations. This is known as large-eddy simulation (LES), as only the “large” scales of turbulence are resolved. This filtering operation results in an extra stress-like term, \(\bm{\tau}^r\), representing the effect of unresolved (or “subgrid” scale) structures in the flow. Denoting the filtering operation by \(\overline \cdot\), the LES governing equations are:

(29)\[ \frac{\partial \bm{\overline q}}{\partial t} + \nabla \cdot \bm{\overline F}(\bm{\overline q}) -S(\bm{\overline q}) = 0 \, , \]

where

(30)\[ \bm{\overline F}(\bm{\overline q}) = \bm{F} (\bm{\overline q}) + \begin{pmatrix} 0\\ \bm{\tau}^r \\ \bm{u} \cdot \bm{\tau}^r \end{pmatrix} \]

More details on deriving the above expression, filtering, and large eddy simulation can be found in [Pop00]. To close the problem, the subgrid stress must be defined. For implicit LES, the subgrid stress is set to zero and the numerical properties of the discretized system are assumed to account for the effect of subgrid scale structures on the filtered solution field. For explicit LES, it is defined by a subgrid stress model.

Data-driven SGS Model

The data-driven SGS model implemented here uses a small neural network to compute the SGS term. The SGS tensor is calculated at nodes using an \(L^2\) projection of the velocity gradient and grid anisotropy tensor, and then interpolated onto quadrature points. More details regarding the theoretical background of the model can be found in [PJE22a] and [PJE22b].

The neural network itself consists of 1 hidden layer and 20 neurons, using Leaky ReLU as its activation function. The slope parameter for the Leaky ReLU function is set via -sgs_model_dd_leakyrelu_alpha. The outputs of the network are assumed to be normalized on a min-max scale, so they must be rescaled by the original min-max bounds. Parameters for the neural network are put into files in a directory found in -sgs_model_dd_parameter_dir. These files store the network weights (w1.dat and w2.dat), biases (b1.dat and b2.dat), and scaling parameters (OutScaling.dat). The first row of each files stores the number of columns and rows in each file. Note that the weight coefficients are assumed to be in column-major order. This is done to keep consistent with legacy file compatibility.

Note

The current data-driven model parameters are not accurate and are for regression testing only.

Differential Filtering

There is the option to filter the solution field using differential filtering. This was first proposed in [Ger86], using an inverse Hemholtz operator. The strong form of the differential equation is

\[ \overline{\phi} - \nabla \cdot (\beta (\bm{D}\bm{\Delta})^2 \nabla \overline{\phi} ) = \phi \]

for \(\phi\) the scalar solution field we want to filter, \(\overline \phi\) the filtered scalar solution field, \(\bm{\Delta} \in \mathbb{R}^{3 \times 3}\) a symmetric positive-definite rank 2 tensor defining the width of the filter, \(\bm{D}\) is the filter width scaling tensor (also a rank 2 SPD tensor), and \(\beta\) is a kernel scaling factor on the filter tensor. This admits the weak form:

\[ \int_\Omega \left( v \overline \phi + \beta \nabla v \cdot (\bm{D}\bm{\Delta})^2 \nabla \overline \phi \right) \,d\Omega - \cancel{\int_{\partial \Omega} \beta v \nabla \overline \phi \cdot (\bm{D}\bm{\Delta})^2 \bm{\hat{n}} \,d\partial\Omega} = \int_\Omega v \phi \, , \; \forall v \in \mathcal{V}_p \]

The boundary integral resulting from integration-by-parts is crossed out, as we assume that \((\bm{D}\bm{\Delta})^2 = \bm{0} \Leftrightarrow \overline \phi = \phi\) at boundaries (this is reasonable at walls, but for convenience elsewhere).

Filter width tensor, Δ

For homogenous filtering, \(\bm{\Delta}\) is defined as the identity matrix.

Note

It is common to denote a filter width dimensioned relative to the radial distance of the filter kernel. Note here we use the filter diameter instead, as that feels more natural (albeit mathematically less convenient). For example, under this definition a box filter would be defined as:

\[ B(\Delta; \bm{r}) = \begin{cases} 1 & \Vert \bm{r} \Vert \leq \Delta/2 \\ 0 & \Vert \bm{r} \Vert > \Delta/2 \end{cases} \]

For inhomogeneous anisotropic filtering, we use the finite element grid itself to define \(\bm{\Delta}\). This is set via -diff_filter_grid_based_width. Specifically, we use the filter width tensor defined in [PJE22b]. For finite element grids, the filter width tensor is most conveniently defined by \(\bm{\Delta} = \bm{g}^{-1/2}\) where \(\bm g = \nabla_{\bm x} \bm{X} \cdot \nabla_{\bm x} \bm{X}\) is the metric tensor.

Filter width scaling tensor, \(\bm{D}\)

The filter width tensor \(\bm{\Delta}\), be it defined from grid based sources or just the homogenous filtering, can be scaled anisotropically. The coefficients for that anisotropic scaling are given by -diff_filter_width_scaling, denoted here by \(c_1, c_2, c_3\). The definition for \(\bm{D}\) then becomes

\[ \bm{D} = \begin{bmatrix} c_1 & 0 & 0 \\ 0 & c_2 & 0 \\ 0 & 0 & c_3 \\ \end{bmatrix} \]

In the case of \(\bm{\Delta}\) being defined as homogenous, \(\bm{D}\bm{\Delta}\) means that \(\bm{D}\) effectively sets the filter width.

The filtering at the wall may also be damped, to smoothly meet the \(\overline \phi = \phi\) boundary condition at the wall. The selected damping function for this is the van Driest function [VD56]:

\[ \zeta = 1 - \exp\left(-\frac{y^+}{A^+}\right) \]

where \(y^+\) is the wall-friction scaled wall-distance (\(y^+ = y u_\tau / \nu = y/\delta_\nu\)), \(A^+\) is some wall-friction scaled scale factor, and \(\zeta\) is the damping coefficient. For this implementation, we assume that \(\delta_\nu\) is constant across the wall and is defined by -diff_filter_friction_length. \(A^+\) is defined by -diff_filter_damping_constant.

To apply this scalar damping coefficient to the filter width tensor, we construct the wall-damping tensor from it. The construction implemented currently limits damping in the wall parallel directions to be no less than the original filter width defined by \(\bm{\Delta}\). The wall-normal filter width is allowed to be damped to a zero filter width. It is currently assumed that the second component of the filter width tensor is in the wall-normal direction. Under these assumptions, \(\bm{D}\) then becomes:

\[ \bm{D} = \begin{bmatrix} \max(1, \zeta c_1) & 0 & 0 \\ 0 & \zeta c_2 & 0 \\ 0 & 0 & \max(1, \zeta c_3) \\ \end{bmatrix} \]

Filter kernel scaling, β

While we define \(\bm{D}\bm{\Delta}\) to be of a certain physical filter width, the actual width of the implied filter kernel is quite larger than “normal” kernels. To account for this, we use \(\beta\) to scale the filter tensor to the appropriate size, as is done in [BJ16]. To match the “size” of a normal kernel to our differential kernel, we attempt to have them match second order moments with respect to the prescribed filter width. To match the box and Gaussian filters “sizes”, we use \(\beta = 1/10\) and \(\beta = 1/6\), respectively. \(\beta\) can be set via -diff_filter_kernel_scaling.

In Situ Machine-Learning Model Training

Training machine-learning models normally uses a priori (already gathered) data stored on disk. This is computationally inefficient, particularly as the scale of the problem grows and the data that is saved to disk reduces to a small percentage of the total data generated by a simulation. One way of working around this to to train a model on data coming from an ongoing simulation, known as in situ (in place) learning.

This is implemented in the code using SmartSim. Briefly, the fluid simulation will periodically place data for training purposes into a database that a separate process uses to train a model. The database used by SmartSim is Redis and the library to connect to the database is called SmartRedis. More information about how to utilize this code in a SmartSim configuration can be found on SmartSim’s website.

To use this code in a SmartSim in situ setup, first the code must be built with SmartRedis enabled. This is done by specifying the installation directory of SmartRedis using the SMARTREDIS_DIR environment variable when building:

make SMARTREDIS_DIR=~/software/smartredis/install

SGS Data-Driven Model In Situ Training

Currently the code is only setup to do in situ training for the SGS data-driven model. Training data is split into the model inputs and outputs. The model inputs are calculated as the same model inputs in the SGS Data-Driven model described earlier. The model outputs (or targets in the case of training) are the subgrid stresses. Both the inputs and outputs are computed from a filtered velocity field, which is calculated via Differential Filtering. The settings for the differential filtering used during training are described in Differential Filtering.

The SGS in situ training can be enabled using the -sgs_train_enable flag. Data can be processed and placed into the database periodically. The interval between is controlled by -sgs_train_write_data_interval. There’s also the choice of whether to add new training data on each database write or to overwrite the old data with new data. This is controlled by -sgs_train_overwrite_data.

The database may also be located on the same node as a MPI rank (collocated) or located on a separate node (distributed). It’s necessary to know how many ranks are associated with each collocated database, which is set by -smartsim_collocated_database_num_ranks.

Advection

A simplified version of system (15), only accounting for the transport of total energy, is given by

(31)\[ \frac{\partial E}{\partial t} + \nabla \cdot (\bm{u} E ) = 0 \, , \]

with \(\bm{u}\) the vector velocity field. In this particular test case, a blob of total energy (defined by a characteristic radius \(r_c\)) is transported by two different wind types.

Rotation

In this case, a uniform circular velocity field transports the blob of total energy. We have solved (31) applying zero energy density \(E\), and no-flux for \(\bm{u}\) on the boundaries.
Translation

In this case, a background wind with a constant rectilinear velocity field, enters the domain and transports the blob of total energy out of the domain.

For the inflow boundary conditions, a prescribed \(E_{wind}\) is applied weakly on the inflow boundaries such that the weak form boundary integral in (19) is defined as

\[ \int_{\partial \Omega_{inflow}} \bm v \cdot \bm{F}(\bm q_N) \cdot \widehat{\bm{n}} \,dS = \int_{\partial \Omega_{inflow}} \bm v \, E_{wind} \, \bm u \cdot \widehat{\bm{n}} \,dS \, , \]

For the outflow boundary conditions, we have used the current values of \(E\), following [PMK92] which extends the validity of the weak form of the governing equations to the outflow instead of replacing them with unknown essential or natural boundary conditions. The weak form boundary integral in (19) for outflow boundary conditions is defined as

\[ \int_{\partial \Omega_{outflow}} \bm v \cdot \bm{F}(\bm q_N) \cdot \widehat{\bm{n}} \,dS = \int_{\partial \Omega_{outflow}} \bm v \, E \, \bm u \cdot \widehat{\bm{n}} \,dS \, , \]

Isentropic Vortex

Three-dimensional Euler equations, which are simplified and nondimensionalized version of system (15) and account only for the convective fluxes, are given by

(32)\[ \begin{aligned} \frac{\partial \rho}{\partial t} + \nabla \cdot \bm{U} &= 0 \\ \frac{\partial \bm{U}}{\partial t} + \nabla \cdot \left( \frac{\bm{U} \otimes \bm{U}}{\rho} + P \bm{I}_3 \right) &= 0 \\ \frac{\partial E}{\partial t} + \nabla \cdot \left( \frac{(E + P)\bm{U}}{\rho} \right) &= 0 \, , \\ \end{aligned} \]

Following the setup given in [ZZS11], the mean flow for this problem is \(\rho=1\), \(P=1\), \(T=P/\rho= 1\) (Specific Gas Constant, \(R\), is 1), and \(\bm{u}=(u_1,u_2,0)\) while the perturbation \(\delta \bm{u}\), and \(\delta T\) are defined as

\[ \begin{aligned} (\delta u_1, \, \delta u_2) &= \frac{\epsilon}{2 \pi} \, e^{0.5(1-r^2)} \, (-\bar{y}, \, \bar{x}) \, , \\ \delta T &= - \frac{(\gamma-1) \, \epsilon^2}{8 \, \gamma \, \pi^2} \, e^{1-r^2} \, , \\ \end{aligned} \]

where \((\bar{x}, \, \bar{y}) = (x-x_c, \, y-y_c)\), \((x_c, \, y_c)\) represents the center of the domain, \(r^2=\bar{x}^2 + \bar{y}^2\), and \(\epsilon\) is the vortex strength (\(\epsilon\) < 10). There is no perturbation in the entropy \(S=P/\rho^\gamma\) (\(\delta S=0)\).

Shock Tube

This test problem is based on Sod’s Shock Tube (from[sod]), a canonical test case for discontinuity capturing in one dimension. For this problem, the three-dimensional Euler equations are formulated exactly as in the Isentropic Vortex problem. The default initial conditions are \(P=1\), \(\rho=1\) for the driver section and \(P=0.1\), \(\rho=0.125\) for the driven section. The initial velocity is zero in both sections. Slip boundary conditions are applied to the side walls and wall boundary conditions are applied at the end walls.

SU upwinding and discontinuity capturing have been implemented into the explicit timestepping operator for this problem. Discontinuity capturing is accomplished using a modified version of the \(YZ\beta\) operator described in [TS07]. This discontinuity capturing scheme involves the introduction of a dissipation term of the form

\[ \int_{\Omega} \nu_{SHOCK} \nabla \bm v \!:\! \nabla \bm q dV \]

The shock capturing viscosity is implemented following the first formulation described in [TS07]. The characteristic velocity \(u_{cha}\) is taken to be the acoustic speed while the reference density \(\rho_{ref}\) is just the local density. Shock capturing viscosity is defined by the following

\[ \nu_{SHOCK} = \tau_{SHOCK} u_{cha}^2 \]

where,

\[ \tau_{SHOCK} = \frac{h_{SHOCK}}{2u_{cha}} \left( \frac{ \,|\, \nabla \rho \,|\, h_{SHOCK}}{\rho_{ref}} \right)^{\beta} \]

\(\beta\) is a tuning parameter set between 1 (smoother shocks) and 2 (sharper shocks. The parameter \(h_{SHOCK}\) is a length scale that is proportional to the element length in the direction of the density gradient unit vector. This density gradient unit vector is defined as \(\hat{\bm j} = \frac{\nabla \rho}{|\nabla \rho|}\). The original formulation of Tezduyar and Senga relies on the shape function gradient to define the element length scale, but this gradient is not available to qFunctions in libCEED. To avoid this problem, \(h_{SHOCK}\) is defined in the current implementation as

\[ h_{SHOCK} = 2 \left( C_{YZB} \,|\, \bm p \,|\, \right)^{-1} \]

where

\[ p_k = \hat{j}_i \frac{\partial \xi_i}{x_k} \]

The constant \(C_{YZB}\) is set to 0.1 for piecewise linear elements in the current implementation. Larger values approaching unity are expected with more robust stabilization and implicit timestepping.

Gaussian Wave

This test case is taken/inspired by that presented in [MDGP+14]. It is intended to test non-reflecting/Riemann boundary conditions. It’s primarily intended for Euler equations, but has been implemented for the Navier-Stokes equations here for flexibility.

The problem has a perturbed initial condition and lets it evolve in time. The initial condition contains a Gaussian perturbation in the pressure field:

\[ \begin{aligned} \rho &= \rho_\infty\left(1+A\exp\left(\frac{-(\bar{x}^2 + \bar{y}^2)}{2\sigma^2}\right)\right) \\ \bm{U} &= \bm U_\infty \\ E &= \frac{p_\infty}{\gamma -1}\left(1+A\exp\left(\frac{-(\bar{x}^2 + \bar{y}^2)}{2\sigma^2}\right)\right) + \frac{\bm U_\infty \cdot \bm U_\infty}{2\rho_\infty}, \end{aligned} \]

where \(A\) and \(\sigma\) are the amplitude and width of the perturbation, respectively, and \((\bar{x}, \bar{y}) = (x-x_e, y-y_e)\) is the distance to the epicenter of the perturbation, \((x_e, y_e)\). The simulation produces a strong acoustic wave and leaves behind a cold thermal bubble that advects at the fluid velocity.

The boundary conditions are freestream in the x and y directions. When using an HLL (Harten, Lax, van Leer) Riemann solver [Tor09] (option -freestream_riemann hll), the acoustic waves exit the domain cleanly, but when the thermal bubble reaches the boundary, it produces strong thermal oscillations that become acoustic waves reflecting into the domain. This problem can be fixed using a more sophisticated Riemann solver such as HLLC [Tor09] (option -freestream_riemann hllc, which is default), which is a linear constant-pressure wave that transports temperature and transverse momentum at the fluid velocity.

Vortex Shedding - Flow past Cylinder

This test case, based on [SHJ91], is an example of using an externally provided mesh from Gmsh. A cylinder with diameter \(D=1\) is centered at \((0,0)\) in a computational domain \(-4.5 \leq x \leq 15.5\), \(-4.5 \leq y \leq 4.5\). We solve this as a 3D problem with (default) one element in the \(z\) direction. The domain is filled with an ideal gas at rest (zero velocity) with temperature 24.92 and pressure 7143. The viscosity is 0.01 and thermal conductivity is 14.34 to maintain a Prandtl number of 0.71, which is typical for air. At time \(t=0\), this domain is subjected to freestream boundary conditions at the inflow (left) and Riemann-type outflow on the right, with exterior reference state at velocity \((1, 0, 0)\) giving Reynolds number \(100\) and Mach number \(0.01\). A symmetry (adiabatic free slip) condition is imposed at the top and bottom boundaries \((y = \pm 4.5)\) (zero normal velocity component, zero heat-flux). The cylinder wall is an adiabatic (no heat flux) no-slip boundary condition. As we evolve in time, eddies appear past the cylinder leading to a vortex shedding known as the vortex street, with shedding period of about 6.

The Gmsh input file, examples/fluids/meshes/cylinder.geo is parametrized to facilitate experimenting with similar configurations. The Strouhal number (nondimensional shedding frequency) is sensitive to the size of the computational domain and boundary conditions.

Forces on the cylinder walls are computed using the “reaction force” method, which is variationally consistent with the volume operator. Given the force components \(\bm F = (F_x, F_y, F_z)\) and surface area \(S = \pi D L_z\) where \(L_z\) is the spanwise extent of the domain, we define the coefficients of lift and drag as

\[ \begin{aligned} C_L &= \frac{2 F_y}{\rho_\infty u_\infty^2 S} \\ C_D &= \frac{2 F_x}{\rho_\infty u_\infty^2 S} \\ \end{aligned} \]

where \(\rho_\infty, u_\infty\) are the freestream (inflow) density and velocity respectively.

Density Current

For this test problem (from [SWW+93]), we solve the full Navier-Stokes equations (15), for which a cold air bubble (of radius \(r_c\)) drops by convection in a neutrally stratified atmosphere. Its initial condition is defined in terms of the Exner pressure, \(\pi(\bm{x},t)\), and potential temperature, \(\theta(\bm{x},t)\), that relate to the state variables via

\[ \begin{aligned} \rho &= \frac{P_0}{( c_p - c_v)\theta(\bm{x},t)} \pi(\bm{x},t)^{\frac{c_v}{ c_p - c_v}} \, , \\ e &= c_v \theta(\bm{x},t) \pi(\bm{x},t) + \bm{u}\cdot \bm{u} /2 + g z \, , \end{aligned} \]

where \(P_0\) is the atmospheric pressure. For this problem, we have used no-slip and non-penetration boundary conditions for \(\bm{u}\), and no-flux for mass and energy densities.

Channel

A compressible channel flow. Analytical solution given in [Whi99]:

\[ u_1 = u_{\max} \left [ 1 - \left ( \frac{x_2}{H}\right)^2 \right] \quad \quad u_2 = u_3 = 0\]

\[T = T_w \left [ 1 + \frac{Pr \hat{E}c}{3} \left \{1 - \left(\frac{x_2}{H}\right)^4 \right \} \right]\]

\[p = p_0 - \frac{2\rho_0 u_{\max}^2 x_1}{Re_H H}\]

where \(H\) is the channel half-height, \(u_{\max}\) is the center velocity, \(T_w\) is the temperature at the wall, \(Pr=\frac{\mu}{c_p \kappa}\) is the Prandlt number, \(\hat E_c = \frac{u_{\max}^2}{c_p T_w}\) is the modified Eckert number, and \(Re_h = \frac{u_{\max}H}{\nu}\) is the Reynolds number.

Boundary conditions are periodic in the streamwise direction, and no-slip and non-penetration boundary conditions at the walls. The flow is driven by a body force determined analytically from the fluid properties and setup parameters \(H\) and \(u_{\max}\).

Flat Plate Boundary Layer

Laminar Boundary Layer - Blasius

Simulation of a laminar boundary layer flow, with the inflow being prescribed by a Blasius similarity solution. At the inflow, the velocity is prescribed by the Blasius soution profile, density is set constant, and temperature is allowed to float. Using weakT: true, density is allowed to float and temperature is set constant. At the outlet, a user-set pressure is used for pressure in the inviscid flux terms (all other inviscid flux terms use interior solution values). The wall is a no-slip, no-penetration, no-heat flux condition. The top of the domain is treated as an outflow and is tilted at a downward angle to ensure that flow is always exiting it.

Turbulent Boundary Layer

Simulating a turbulent boundary layer without modeling the turbulence requires resolving the turbulent flow structures. These structures may be introduced into the simulations either by allowing a laminar boundary layer naturally transition to turbulence, or imposing turbulent structures at the inflow. The latter approach has been taken here, specifically using a synthetic turbulence generation (STG) method.

Synthetic Turbulence Generation (STG) Boundary Condition

We use the STG method described in [SSST14]. Below follows a re-description of the formulation to match the present notation, and then a description of the implementation and usage.

Equation Formulation

\[ \bm{u}(\bm{x}, t) = \bm{\overline{u}}(\bm{x}) + \bm{C}(\bm{x}) \cdot \bm{v}' \]

\[ \begin{aligned} \bm{v}' &= 2 \sqrt{3/2} \sum^N_{n=1} \sqrt{q^n(\bm{x})} \bm{\sigma}^n \cos(\kappa^n \bm{d}^n \cdot \bm{\hat{x}}^n(\bm{x}, t) + \phi^n ) \\ \bm{\hat{x}}^n &= \left[(x - U_0 t)\max(2\kappa_{\min}/\kappa^n, 0.1) , y, z \right]^T \end{aligned} \]

Here, we define the number of wavemodes \(N\), set of random numbers \( \{\bm{\sigma}^n, \bm{d}^n, \phi^n\}_{n=1}^N\), the Cholesky decomposition of the Reynolds stress tensor \(\bm{C}\) (such that \(\bm{R} = \bm{CC}^T\) ), bulk velocity \(U_0\), wavemode amplitude \(q^n\), wavemode frequency \(\kappa^n\), and \(\kappa_{\min} = 0.5 \min_{\bm{x}} (\kappa_e)\).

\[ \kappa_e = \frac{2\pi}{\min(2d_w, 3.0 l_t)} \]

where \(l_t\) is the turbulence length scale, and \(d_w\) is the distance to the nearest wall.

The set of wavemode frequencies is defined by a geometric distribution:

\[ \kappa^n = \kappa_{\min} (1 + \alpha)^{n-1} \ , \quad \forall n=1, 2, ... , N \]

The wavemode amplitudes \(q^n\) are defined by a model energy spectrum \(E(\kappa)\):

\[ q^n = \frac{E(\kappa^n) \Delta \kappa^n}{\sum^N_{n=1} E(\kappa^n)\Delta \kappa^n} \ ,\quad \Delta \kappa^n = \kappa^n - \kappa^{n-1} \]

\[ E(\kappa) = \frac{(\kappa/\kappa_e)^4}{[1 + 2.4(\kappa/\kappa_e)^2]^{17/6}} f_\eta f_{\mathrm{cut}} \]

\[ f_\eta = \exp \left[-(12\kappa /\kappa_\eta)^2 \right], \quad f_\mathrm{cut} = \exp \left( - \left [ \frac{4\max(\kappa-0.9\kappa_\mathrm{cut}, 0)}{\kappa_\mathrm{cut}} \right]^3 \right) \]

\(\kappa_\eta\) represents turbulent dissipation frequency, and is given as \(2\pi (\nu^3/\varepsilon)^{-1/4}\) with \(\nu\) the kinematic viscosity and \(\varepsilon\) the turbulent dissipation. \(\kappa_\mathrm{cut}\) approximates the effective cutoff frequency of the mesh (viewing the mesh as a filter on solution over \(\Omega\)) and is given by:

\[ \kappa_\mathrm{cut} = \frac{2\pi}{ 2\min\{ [\max(h_y, h_z, 0.3h_{\max}) + 0.1 d_w], h_{\max} \} } \]

The enforcement of the boundary condition is identical to the blasius inflow; it weakly enforces velocity, with the option of weakly enforcing either density or temperature using the the -weakT flag.

Initialization Data Flow

Data flow for initializing function (which creates the context data struct) is given below:

flowchart LR subgraph STGInflow.dat y lt[l_t] eps Rij[R_ij] ubar end subgraph STGRand.dat rand[RN Set]; end subgraph User Input u0[U0]; end subgraph init[Create Context Function] ke[k_e] N; end lt --Calc-->ke --Calc-->kn y --Calc-->ke subgraph context[Context Data] yC[y] randC[RN Set] Cij[C_ij] u0 --Copy--> u0C[U0] kn[k^n]; ubarC[ubar] ltC[l_t] epsC[eps] end ubar --Copy--> ubarC; y --Copy--> yC; lt --Copy--> ltC; eps --Copy--> epsC; rand --Copy--> randC; rand --> N --Calc--> kn; Rij --Calc--> Cij[C_ij]

This is done once at runtime. The spatially-varying terms are then evaluated at each quadrature point on-the-fly, either by interpolation (for \(l_t\), \(\varepsilon\), \(C_{ij}\), and \(\overline{\bm u}\)) or by calculation (for \(q^n\)).

The STGInflow.dat file is a table of values at given distances from the wall. These values are then interpolated to a physical location (node or quadrature point). It has the following format:

[Total number of locations] 14
[d_w] [u_1] [u_2] [u_3] [R_11] [R_22] [R_33] [R_12] [R_13] [R_23] [sclr_1] [sclr_2] [l_t] [eps]

where each [ ] item is a number in scientific notation (ie. 3.1415E0), and sclr_1 and sclr_2 are reserved for turbulence modeling variables. They are not used in this example.

The STGRand.dat file is the table of the random number set, \(\{\bm{\sigma}^n, \bm{d}^n, \phi^n\}_{n=1}^N\). It has the format:

[Number of wavemodes] 7
[d_1] [d_2] [d_3] [phi] [sigma_1] [sigma_2] [sigma_3]

The following table is presented to help clarify the dimensionality of the numerous terms in the STG formulation.

Math	Label	\(f(\bm{x})\)?	\(f(n)\)?
\( \{\bm{\sigma}^n, \bm{d}^n, \phi^n\}_{n=1}^N\)	RN Set	No	Yes
\(\bm{\overline{u}}\)	ubar	Yes	No
\(U_0\)	U0	No	No
\(l_t\)	l_t	Yes	No
\(\varepsilon\)	eps	Yes	No
\(\bm{R}\)	R_ij	Yes	No
\(\bm{C}\)	C_ij	Yes	No
\(q^n\)	q^n	Yes	Yes
\(\{\kappa^n\}_{n=1}^N\)	k^n	No	Yes
\(h_i\)	h_i	Yes	No
\(d_w\)	d_w	Yes	No

Internal Damping Layer (IDL)

The STG inflow boundary condition creates large amplitude acoustic waves. We use an internal damping layer (IDL) to damp them out without disrupting the synthetic structures developing into natural turbulent structures. This implementation was inspired from [SSST14], but is implemented here as a ramped volumetric forcing term, similar to a sponge layer (see 8.4.2.4 in [Col23] for example). It takes the following form:

\[ S(\bm{q}) = -\sigma(\bm{x})\left.\frac{\partial \bm{q}}{\partial \bm{Y}}\right\rvert_{\bm{q}} \bm{Y}' \]

where \(\bm{Y}' = [P - P_\mathrm{ref}, \bm{0}, 0]^T\), and \(\sigma(\bm{x})\) is a linear ramp starting at -idl_start with length -idl_length and an amplitude of inverse -idl_decay_rate. The damping is defined in terms of a pressure-primitive anomaly \(\bm Y'\) converted to conservative source using \(\partial \bm{q}/\partial \bm{Y}\rvert_{\bm{q}}\), which is linearized about the current flow state. \(P_\mathrm{ref}\) is defined via the -reference_pressure flag.

Meshing

The flat plate boundary layer example has custom meshing features to better resolve the flow when using a generated box mesh. These meshing features modify the nodal layout of the default, equispaced box mesh and are enabled via -mesh_transform platemesh. One of those is tilting the top of the domain, allowing for it to be a outflow boundary condition. The angle of this tilt is controlled by -platemesh_top_angle.

The primary meshing feature is the ability to grade the mesh, providing better resolution near the wall. There are two methods to do this; algorithmically, or specifying the node locations via a file. Algorithmically, a base node distribution is defined at the inlet (assumed to be \(\min(x)\)) and then linearly stretched/squeezed to match the slanted top boundary condition. Nodes are placed such that -platemesh_Ndelta elements are within -platemesh_refine_height of the wall. They are placed such that the element height matches a geometric growth ratio defined by -platemesh_growth. The remaining elements are then distributed from -platemesh_refine_height to the top of the domain linearly in logarithmic space.

Alternatively, a file may be specified containing the locations of each node. The file should be newline delimited, with the first line specifying the number of points and the rest being the locations of the nodes. The node locations used exactly at the inlet (assumed to be \(\min(x)\)) and linearly stretched/squeezed to match the slanted top boundary condition. The file is specified via -platemesh_y_node_locs_path. If this flag is given an empty string, then the algorithmic approach will be performed.

Taylor-Green Vortex

This problem is really just an initial condition, the Taylor-Green Vortex:

\[ \begin{aligned} u &= V_0 \sin(\hat x) \cos(\hat y) \sin(\hat z) \\ v &= -V_0 \cos(\hat x) \sin(\hat y) \sin(\hat z) \\ w &= 0 \\ p &= p_0 + \frac{\rho_0 V_0^2}{16} \left ( \cos(2 \hat x) + \cos(2 \hat y)\right) \left( \cos(2 \hat z) + 2 \right) \\ \rho &= \frac{p}{R T_0} \\ \end{aligned} \]

where \(\hat x = 2 \pi x / L\) for \(L\) the length of the domain in that specific direction. This coordinate modification is done to transform a given grid onto a domain of \(x,y,z \in [0, 2\pi)\).

This initial condition is traditionally given for the incompressible Navier-Stokes equations. The reference state is selected using the -reference_{velocity,pressure,temperature} flags (Euclidean norm of -reference_velocity is used for \(V_0\)).