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`	Run in test mode	`false`
`-compare_final_state_atol`	Test absolute tolerance	`1E-11`
`-compare_final_state_filename`	Test filename
`-problem`	Problem to solve (`advection`, `advection2d`, `density_current`, or `euler_vortex`)	`density_current`
`-implicit`	Use implicit time integartor formulation
`-degree`	Polynomial degree of tensor product basis (must be >= 1)	`1`
`-q_extra`	Number of extra quadrature points	`2`
`-viz_refine`	Use regular refinement for visualization	`0`
`-output_freq`	Frequency of output, in number of steps. `0` has no output, `-1` outputs final state only	`10`
`-continue`	Continue from previous solution	`0`
`-output_dir`	Output directory	`.`
`-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
`-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 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 2D 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

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)	`shpere`
`-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, \(C_v\)	`36.0`
`-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)`
`-g`	Gravitational acceleration	`9.81`	`m/s^2`
`-lambda`	Stokes hypothesis second viscosity coefficient	`-2/3`
`-mu`	Shear dynamic viscosity coefficient	`75`	`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

Density current¶

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

Table 9 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 the following command-line options are available in addition to the Newtonian Ideal Gas options:

Table 10 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

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 the following command-line options are available in addition to the Newtonian Ideal Gas options:

Table 11 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_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`
`-stg_use`	Whether to use stg for the inflow conditions	`false`
`-platemesh_y_node_locs_path`	Path to file with y node locations. If empty, will use mesh warping instead.	`""`
`-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: 0.2e-5
  max_time: 1.0e-3
output_freq: 10

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

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

stab: 'supg'
Ctau_t: 1
#Ctau_v: 36,60,128 is what PHASTA has for p=1,2,3
# Linear Settings:
Ctau_v: 36
Ctau_C: 0.25
Ctau_M: 0.25
Ctau_E: 0.125
# # Quadratic Settings:
# Ctau_v: 60
# Ctau_C: 0.125
# Ctau_M: 0.125
# Ctau_E: 0.125

q_extra: 0

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
g: 0,0,0

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

STG Inflow for Flat Plate¶

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

Table 12 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`

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 [GRL10], cf. SE3) is given in what follows. The compressible Navier-Stokes equations in conservative form are

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

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), \(\bm{I}_3\) represents the \(3 \times 3\) identity matrix, \(g\) the gravitational acceleration constant, \(\bm{\hat{k}}\) the unit vector in the \(z\) direction, \(k\) the thermal conductivity constant, \(T\) represents the temperature, and \(P\) the pressure, given by the following equation of state

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

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

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 \(\psi_{kji} = h_i(X_0)h_j(X_1)h_k(X_2)\).

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

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 \(\bm q_N\):

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

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 (19) will correspond to a weak form, as explained below. In determining how difficult a given problem is to solve, we consider the Jacobian of (19),

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

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.

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,

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

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.

We solve (20) 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 (20). The weak form for this method is given as

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

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

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

In both (22) and (21), \(\mathcal P\) is called the perturbation to the test-function space, since it modifies the original Galerkin method into SUPG or SU schemes. It is defined as

(23)¶\[ \mathcal P(\bm v) \equiv \bm{\tau} \left(\frac{\partial \bm{F}_{\text{adv}} (\bm{q}_N)}{\partial \bm{q}_N} \right) \, \nabla \bm v\,, \]

where parameter \(\bm{\tau} \in \mathbb R^{3}\) (spatial index) or \(\bm \tau \in \mathbb R^{5\times 5}\) (field indices) is an intrinsic time scale matrix. Most generally, we consider \(\bm\tau \in \mathbb R^{3,5,5}\). This expression contains the advective flux Jacobian, which may be thought of as mapping from a 5-vector (state) to a \((5,3)\) tensor (flux) or from a \((5,3)\) tensor (gradient of state) to a 5-vector (time derivative of state); the latter is used in (23) because it’s applied to \(\nabla\bm v\). 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). This action is also readily computed by forward-mode AD, but since \(\bm v\) is a test function, we actually need the action of the adjoint to use (23) in finite element computation; that can be computed by reverse-mode AD. We may equivalently write the stabilization term as

\[ \mathcal P(\bm v)^T \bm r = \nabla \bm v \tcolon \left(\frac{\partial \bm F_{\text{adv}}}{\partial \bm q}\right)^T \, \bm\tau \bm r, \]

where \(\bm r\) is the strong form residual and \(\bm\tau\) is a \(5\times 5\) matrix.

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 Density Current problem.

Advection¶

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

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

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 (30) 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 (20) 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 (20) 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

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

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 {cite} tezduyar2007yzb. 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.

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

Meshing¶

The flat plate boundary layer example has custom meshing features to better resolve the flow. 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 controled 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.