Compressible NavierStokes miniapp
This example is located in the subdirectory examples/fluids
.
It solves the timedependent NavierStokes equations of compressible gas dynamics in a static Eulerian threedimensional frame using unstructured highorder finite/spectral element spatial discretizations and explicit or implicit highorder timestepping (available in PETSc).
Moreover, the NavierStokes 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 miniapp
The NavierStokes miniapp is controlled via commandline options. The following options are common among all problem types:
Option 
Description 
Default value 


CEED resource specifier 


Run in test mode and specify whether solution ( 


Test absolute tolerance 


Test filename 


Problem to solve ( 


Use implicit time integrator formulation 


Polynomial degree of tensor product basis (must be >= 1) 


Number of extra quadrature points 


PETSc output format, such as 


Number of time steps between visualization output frames. 


Number of frames written per CGNS file if the CGNS file name includes a format specifier ( 


Number of steps between writing binary checkpoints. 


Checkpoints include VTK ( 


Use regular refinement for VTK visualization 


Output directory for binary checkpoints and VTK files (if enabled). 


Whether to add step numbers to output binary files 


Continue from previous solution (input is step number of previous solution) 


Path to solution binary file from which to continue from 


Path to time stamp binary file (only for legacy checkpoints) 


Use wall boundary conditions on this list of faces 


An array of constrained component numbers for wall BCs 


Use slip boundary conditions, for the x component, on this list of faces 


Use slip boundary conditions, for the y component, on this list of faces 


Use slip boundary conditions, for the z component, on this list of faces 


Use inflow boundary conditions on this list of faces 


Use outflow boundary conditions on this list of faces 


Use freestream boundary conditions on this list of faces 


Number of timesteps between statistics collection 


Sets the PetscViewer for the statistics file writing, such as 


Number of timesteps between statistics file writing ( 


Number of frames written per CGNS file if the CGNS file name includes a format specifier ( 


Viewer for the force on each noslip wall, e.g., 


Transform the mesh, usually for an initial box mesh. 


View PETSc 


View PETSc performance log 


View comprehensive information about runtime 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:
PETSc Face Name 
Cartesian direction 
Face ID 

faceMarkerBottom 
z 
1 
faceMarkerRight 
+x 
2 
faceMarkerTop 
+z 
3 
faceMarkerLeft 
x 
4 
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 gridscale 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 illposed 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 PHASTAC, 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 cellbased 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 Zordering 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” \(E\). The advection problems can be run in both 2D and 3D, based on the DM defined for the problem. The following additional commandline options are available:
Option 
Description 
Default value 
Unit 


Characteristic radius of thermal bubble 



1 meter in scaled length units 



1 second in scaled time units 



1 kilogram in scaled mass units 



Strong (1) or weak/integrated by parts (0) residual 



Stabilization method ( 



Scale coefficient for stabilization tau (nondimensional) 



Wind type in Advection ( 



Constant wind vector when 



Total energy of inflow wind when 



Initial condition type, from 



Different shapes for 

For 3D advection, 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
For 2D advection, an example of the rotation
mode can be run with:
./navierstokes problem advection 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 advection dm_plex_box_faces 20,20 dm_plex_box_lower 0,0 dm_plex_box_upper 1000,1000 units_meter 1e4 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
.
Inviscid Ideal Gas
Isentropic Euler vortex
For the Isentropic Vortex problem, the following additional commandline options are available:
Option 
Description 
Default value 
Unit 


Location of vortex center 



1 meter in scaled length units 



1 second in scaled time units 



Background velocity vector 



Strength of vortex < 10 



Stabilization constant 

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 commandline options are available:
Option 
Description 
Default value 
Unit 


1 meter in scaled length units 



1 second in scaled time units 



Use YZB discontinuity capturing 



Stabilization method ( 

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 commandline options are available:
Option 
Description 
Default value 
Unit 


1 meter in scaled length units 



1 second in scaled time units 



1 kilogram in scaled mass units 



1 Kelvin in scaled temperature units 



Stabilization method ( 



Stabilization constant, \(c_\tau\) 



Stabilization time constant, \(C_t\) 



Stabilization viscous constant, \(C_v\) 



Stabilization continuity constant, \(C_c\) 



Stabilization momentum constant, \(C_m\) 



Stabilization energy constant, \(C_E\) 



Heat capacity at constant volume 



Heat capacity at constant pressure 



Gravitational acceleration vector 



Stokes hypothesis second viscosity coefficient 



Shear dynamic viscosity coefficient 



Thermal conductivity 



Developer option to test properties 

boolean 

State variables to solve solution with. 

string 

Characteristic timescale of the pressure deviance decay. The timestep is good starting point 



Start of IDL in the x direction 



Length of IDL in the positive x direction 



Type of subgrid stress model to use. Currently only 

string 

Slope parameter for Leaky ReLU activation function. 
0 


Path to directory with datadriven model parameters (weights, biases, etc.) 

string 

Enable differential filter TSMonitor 

boolean 

Use filter width based on the grid size 

boolean 

Anisotropic scaling for filter width in wallaligned coordinates (snz) 



Scaling to make differential kernel size equivalent to other filter kernels 



Damping function to use at the wall for anisotropic filtering ( 

string 

Constant for the walldamping function. \(A^+\) for 
25 


Friction length associated with the flow, \(\delta_\nu\). Used in walldamping functions 
0 


Whether to enable in situ training of datadriven SGS model. Require building with SmartRedis. 

boolean 

Number of timesteps between writing training data into SmartRedis database 



Whether new training data should overwrite old data on database 

boolean 

Number of MPI ranks associated with each collocated database (i.e. ranks per node) 

Gaussian Wave
The Gaussian wave problem has the following commandline options in addition to the Newtonian Ideal Gas options:
Option 
Description 
Default value 
Unit 


Riemann solver for boundaries (HLL or HLLC) 



Freestream velocity vector 



Freestream temperature 



Freestream pressure 



Coordinates of center of perturbation 



Amplitude of the perturbation 



Width parameter of the perturbation 


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: 2e3
type: alpha
alpha_radius: 0.5
#monitor_solution: cgns:nwave.cgns
#monitor_solution_interval: 10
implicit: true
stab: supg
state_var: primitive
snes_rtol: 1e4
ksp_rtol: 1e2
snes_lag_jacobian: 20
snes_lag_jacobian_persists:
## Demonstrate acoustic wave dissipation using an internal damping layer
# idl:
# decay_time: 2e3
# start: 0
# length: .25
Vortex Shedding  Flow past Cylinder
The vortex shedding, flow past cylinder problem has the following commandline options in addition to the Newtonian Ideal Gas options:
Option 
Description 
Default value 
Unit 


Freestream velocity vector 



Freestream temperature 



Freestream pressure 


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/fluidsnavierstokes
$ mpiexec n 6 build/fluidsnavierstokes 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:vortexsheddingq3g1n08.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/cylinderq1n08.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 commandline options in addition to the Newtonian Ideal Gas options:
Option 
Description 
Default value 
Unit 


Location of bubble center 



Axis of density current cylindrical anomaly, or 



Characteristic radius of thermal bubble 



Reference potential temperature 



Perturbation of potential temperature 



Atmospheric pressure 



BruntVaisala frequency 


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 commandline options in addition to the Newtonian Ideal Gas options:
Option 
Description 
Default value 
Unit 


Maximum/centerline velocity of the flow 



Reference potential temperature 



Atmospheric pressure 



Multiplier for body force ( 
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: 5e6
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 commandline options in addition to the Newtonian Ideal Gas options:
Option 
Description 
Default value 
Unit 


Freestream velocity 



Freestream temperature 



Wall temperature 



Boundary layer height at the inflow 



Atmospheric pressure 



Whether to modify the mesh using the given options below. 



Height at which 



Number of elements to keep below 



Growth rate of the elements in the refinement region 



Downward angle of the top face of the domain. This face serves as an outlet. 



Path to file with y node locations. If empty, will use mesh warping instead. 



Whether to use STG for the inflow conditions 



Number of Chebyshev terms 



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: 2e6
max_time: 1.0e3
#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: 4.2e3,4.2e3,5.e5
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 commandline options:
Option 
Description 
Default value 
Unit 


Path to the STGInflow file 



Path to the STGRand file 



Growth rate of the wavemodes 



Convective velocity, \(U_0\) 



Only impose the mean velocity (no fluctutations) 



Strongly enforce the STG inflow boundary condition 



“Extrude” the fluctuations through the domain as an initial condition 

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 NavierStokes equations
The mathematical formulation (from [SHJ91]) is given in what follows. The compressible NavierStokes equations in conservative form are
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
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
for the state variables 5dimensional vector
where the flux and the source terms, respectively, are given by
Finite Element Formulation (Spatial Discretization)
Let the discrete solution be
with \(P=p+1\) the number of nodes in the element \(e\). We use tensorproduct 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,
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,
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 timestepping method
The following explicit formulation is solved with the adaptive RungeKuttaFehlberg (RKF45) method by default (any explicit timestepping scheme available in PETSc can be chosen at runtime)
where
and with
Implicit timestepping 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 timestepping scheme available in PETSc can be chosen at runtime).
The implicit formulation solves nonlinear systems for \(\bm q_N\):
where the time derivative \(\bm{\dot q}_N\) is defined by
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 RungeKutta, 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),
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 wellconditioned 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 timeaccurate 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 realworld flows.
Galerkin methods produce oscillations for transportdominated 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 (lowviscosity/poorly resolved) NavierStokes, in which case stabilization is necessary. Our formulation follows [HST10], which offers a comprehensive review of stabilization and shockcapturing methods for continuous finite element discretization of compressible flows.
SUPG (streamlineupwind/PetrovGalerkin)
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 (streamlineupwind)
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)
where \(\diff P\) is defined by differentiating (16).
Stabilization scale \(\bm\tau\)
A velocity vector \(\bm u\) can be pulled back to the reference element as \(\bm u_{\bm X} = \nabla_{\bm x}\bm X \cdot \bm u\), with units of reference length (nondimensional) per second. To build intuition, consider a boundary layer element of dimension \((1, \epsilon)\), for which \(\nabla_{\bm x} \bm X = \bigl(\begin{smallmatrix} 2 & \\ & 2/\epsilon \end{smallmatrix}\bigr)\). So a small normal component of velocity will be amplified (by a factor of the aspect ratio \(1/\epsilon\)) in this transformation. The ratio \(\lVert \bm u \rVert / \lVert \bm u_{\bm X} \rVert\) is a covariant measure of (half) the element length in the direction of the velocity. A contravariant measure of element length in the direction of a unit vector \(\hat{\bm n}\) is given by \(\lVert \bigl(\nabla_{\bm X} \bm x\bigr)^T \hat{\bm n} \rVert\). While \(\nabla_{\bm X} \bm x\) is readily computable, its inverse \(\nabla_{\bm x} \bm X\) is needed directly in finite element methods and thus more convenient for our use. If we consider a parallelogram, the covariant measure is larger than the contravariant measure for vectors pointing between acute corners and the opposite holds for vectors between oblique corners.
The cell Péclet number is classically defined by \(\mathrm{Pe}_h = \lVert \bm u \rVert h / (2 \kappa)\) where \(\kappa\) is the diffusivity (units of \(m^2/s\)). This can be generalized to arbitrary grids by defining the local Péclet number
For scalar advectiondiffusion, the stabilization is a scalar
where \(\xi(\mathrm{Pe}) = \coth \mathrm{Pe}  1/\mathrm{Pe}\) approaches 1 at large local Péclet number. Note that \(\tau\) has units of time and, in the transportdominated limit, is proportional to element transit time in the direction of the propagating wave. For advectiondiffusion, \(\bm F(q) = \bm u q\), and thus the SU stabilization term is
where the term in parentheses is a rank1 diffusivity tensor that has been pulled back to the reference element. See [HST10] equations 1517 and 3436 for further discussion of this formulation.
For the NavierStokes and Euler equations, [WJD03] defines a \(5\times 5\) diagonal stabilization \(\mathrm{diag}(\tau_c, \tau_m, \tau_m, \tau_m, \tau_E)\) consisting of
continuity stabilization \(\tau_c\)
momentum stabilization \(\tau_m\)
energy stabilization \(\tau_E\)
The NavierStokes code in this example uses the following formulation for \(\tau_c\), \(\tau_m\), \(\tau_E\):
where \(\bm g = \nabla_{\bm x} \bm{X}^T \cdot \nabla_{\bm x} \bm{X}\) is the metric tensor and \(\Vert \cdot \Vert_F\) is the Frobenius norm. This formulation is currently not available in the Euler code.
In the Euler code, we follow [HST10] in defining a \(3\times 3\) diagonal stabilization according to spatial criterion 2 (equation 27) as follows.
where \(c_{\tau}\) is a multiplicative constant reported to be optimal at 0.5 for linear elements, \(\hat{\bm n}_i\) is a unit vector in direction \(i\), and \(\nabla_{x_i} = \hat{\bm n}_i \cdot \nabla_{\bm x}\) is the derivative in direction \(i\). The flux Jacobian \(\frac{\partial \bm F_{\text{adv}}}{\partial \bm q} \cdot \hat{\bm n}_i\) in each direction \(i\) is a \(5\times 5\) matrix with spectral radius \((\lambda_{\max \text{abs}})_i\) equal to the fastest wave speed. The complete set of eigenvalues of the Euler flux Jacobian in direction \(i\) are (e.g., [Tor09])
where \(u_i = \bm u \cdot \hat{\bm n}_i\) is the velocity component in direction \(i\) and \(a = \sqrt{\gamma P/\rho}\) is the sound speed for ideal gasses. Note that the first and last eigenvalues represent nonlinear acoustic waves while the middle three are linearly degenerate, carrying a contact wave (temperature) and transverse components of momentum. The fastest wave speed in direction \(i\) is thus
Note that this wave speed is specific to ideal gases as \(\gamma\) is an ideal gas parameter; other equations of state will yield a different acoustic wave speed.
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 underresolved (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 NavierStokes equations. This is known as largeeddy simulation (LES), as only the “large” scales of turbulence are resolved. This filtering operation results in an extra stresslike 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:
where
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.
Datadriven SGS Model
The datadriven 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 minmax scale, so they must be rescaled by the original minmax 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 columnmajor order.
This is done to keep consistent with legacy file compatibility.
Note
The current datadriven 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
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 positivedefinite 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:
The boundary integral resulting from integrationbyparts 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:
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
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]:
where \(y^+\) is the wallfriction scaled walldistance (\(y^+ = y u_\tau / \nu = y/\delta_\nu\)), \(A^+\) is some wallfriction 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 walldamping 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 wallnormal 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 wallnormal direction. Under these assumptions, \(\bm{D}\) then becomes:
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 MachineLearning Model Training
Training machinelearning 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 DataDriven Model In Situ Training
Currently the code is only setup to do in situ training for the SGS datadriven model. Training data is split into the model inputs and outputs. The model inputs are calculated as the same model inputs in the SGS DataDriven 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
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 noflux 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
Threedimensional Euler equations, which are simplified and nondimensionalized version of system (15) and account only for the convective fluxes, are given by
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
where \((\bar{x}, \, \bar{y}) = (xx_c, \, yy_c)\), \((x_c, \, y_c)\) 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 threedimensional 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
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
where,
\(\beta\) 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
where
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 nonreflecting/Riemann boundary conditions. It’s primarily intended for Euler equations, but has been implemented for the NavierStokes 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:
where \(A\) and \(\sigma\) are the amplitude and width of the perturbation, respectively, and \((\bar{x}, \bar{y}) = (xx_e, yy_e)\) 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 constantpressure 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 Riemanntype 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 heatflux). The cylinder wall is an adiabatic (no heat flux) noslip 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
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 NavierStokes 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
where \(P_0\) is the atmospheric pressure. For this problem, we have used noslip and nonpenetration boundary conditions for \(\bm{u}\), and noflux for mass and energy densities.
Channel
A compressible channel flow. Analytical solution given in [Whi99]:
where \(H\) is the channel halfheight, \(u_{\max}\) 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 noslip and nonpenetration 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 userset
pressure is used for pressure in the inviscid flux terms (all other inviscid
flux terms use interior solution values). The wall is a noslip,
nopenetration, noheat 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 redescription of the formulation to match the present notation, and then a description of the implementation and usage.
Equation Formulation
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 \(\kappa_{\min} = 0.5 \min_{\bm{x}} (\kappa_e)\).
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:
The wavemode amplitudes \(q^n\) are defined by a model energy spectrum \(E(\kappa)\):
\(\kappa_\eta\) 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:
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:
This is done once at runtime. The spatiallyvarying terms are then evaluated at each quadrature point onthefly, 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:
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 pressureprimitive
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.
TaylorGreen Vortex
This problem is really just an initial condition, the TaylorGreen Vortex:
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 NavierStokes equations.
The reference state is selected using the reference_{velocity,pressure,temperature}
flags (Euclidean norm of reference_velocity
is used for \(V_0\)).