User Guide

How to Run

pyBaram provides a console script, which uses argparse module. When you run pybaram, following help output is given:

user@Computer ~/pyBaram$ pybaram

usage: pybaram [-h] [--verbose] {import,partition,run,restart,export} ...

positional arguments:
{import,partition,run,restart,export}
                        sub-command help
    import              import --help
    partition           partition --help
    run                 run --help
    restart             run --help
    export              export --help

optional arguments:
-h, --help            show this help message and exit
--verbose, -v

pybaram import — Convert the mesh generator output to pyBaram mesh file (.pbrm). pyBaram can convert CGNS mesh (.cgns) file or Gmsh mesh file (.msh)

Example:
```
user@Computer ~/pyBaram$ pybaram import mesh.cgns mesh.pbrm
```
pybaram partition — Partition mesh file for MPI parallel computation. Currently, unsplitted mesh file can be partitioned.

Example:
```
user@Computer ~/pyBaram$ pybaram partition 2 mesh.pbrm mesh_p2.pbrm
```
pybaram run — Conduct flow simulation with a given mesh and configuration files (.ini).

Example:
```
user@Computer ~/pyBaram$ pybaram run mesh.pbrm conf.ini
```
If you would like conduct MPI parallel computation, please use mpirun -n <cores> to launch pybaram script. Note that the mesh file should be partitioned by the same number of cores.

Example:
```
user@Computer ~/pyBaram$ mpirun -np 2 pybaram run mesh_p2.pbrm conf.ini
```
pybaram restart — Restart flow simulation with a given mesh and solution files. If you would like to restart with different methods, please append the configuration file.

Example:
```
user@Computer ~/pyBaram$ pybaram restart mesh.pbrm sol-100.pbrs
```
pybaram export — Convert solution files to VTK unstructured file (.vtu) or Tecplot data file (.plt).

Example:
```
user@Computer ~/pyBaram$ pybaram export mesh.pbrm sol-100.pbrs out.vtu
```

Mesh File

pyBaram can handle unstructured mixed elements; however, there are some cautions. Currently, only a single unstructured zone can be solved. It is important that volumes and faces are appropriately labeled. The volume label for a single zone should be set as fluid, and faces assigned for boundary conditions must have distinct labels.

Configuration File

The parameters for pyBaram simulation are specified in the configuration file. This file is written in the INI file format, and it is parsed using the configparser module. The following sections provide details on the sections and parameters.

Backends

The backend section configures how to run pybaram. Currently, pybaram can be running on CPU and there is only ‘backend-cpu’ section.

[backend-cpu]

Parameterize cpu backend with

multi-thread — for selecting the multi-threading layer. This parameter passes to Numba.
single | parallel | omp | tbb

where
single — use only one thread for the program. It is default value. If you are running with only MPI parallel computation, please use it. Some numerical schemes only support single thread option.

parallel — use the default multi-threading layer of Numba. Depending on the libraries, omp or tbb is used.

omp — use OpenMP multi-threading layer.

tbb — use Intel Threading building Blocks multi-threading layer.

Example:

[backend-cpu]
multi-thread = parallel

Constants

In the constants section, essential and user-defined constants are configured. Some constants can be expressed as a function of other constants. Followings are the essential constant depending on the equation to solve.

gamma — ratio of the specific heats. For conventional air, $\gamma=1.4$ . All compressible equations need it.

float
mu — dynamic viscosity. It should be defined for constant viscosity.

float
Pr — Prandtl number. It should be defined for viscous simulation. For conventional air, $Pr=0.72$ .

float
Prt — Turbulent Prandtl number. It should be defined for turbulent simulation. For conventional air, $Prt=0.9$ .

float

Example:

[constants]
gamma = 1.4
Pr = 0.72
Prt = 0.9
Re = 6.5e6
mach = 0.729
rhof = 1.0
uf = %(mach)s
pf = 1/%(gamma)s
mu = %(mach)s/%(Re)s
nutf = 4*%(mu)s/%(rhof)s

Solvers

In following sections, numerical schemes are configured.

[solver]

Type of equations and spatial discretization schemes are configured as follows.

system — type of equations.
euler | navier-stokes | rans-sa | rans-kwsst
- rans- model — Reynolds-averaged Navier-Stokes equation with turbulence model.
  rans-sa — one equation Spalart-Allmaras model
  
  rans-kwsst — two-equation $k\omega$ -SST model
order — spatial order of accuracy.

1 | 2
gradient —- method to calculate gradient. The default value is hybrid.

hybrid | least-square | weighted-least-square | green-gauss
limiter — slope limiter for shock-capturing. It is configured only if the order is 2. Default value is none.

none | mlp-u1 | mlp-u2
u2k — tuning parameter for MLP-u2 limiter. Normally it is $O(1)$ .

float
riemann-solver — scheme to compute inviscid flux at interface.

rusanov | roe | roem | rotated-roem | hllem | ausmpw+ | ausm+up
viscosity — method to compute viscosity. Default value is constant.

constant | sutherland

Example:

[solver]
system = rans-kwsst
order = 2
limiter = mlp-u2
u2k = 5.0
riemann-solver = ausmpw+
viscosity = sutherland

[solver-viscosity-sutherland]

The parameters associated with Sutherland’s law can be configured as follows:

muref — Reference viscosity of the problem. See the note

float
Tref — Reference temperature of the problem. This is a dimensional unit.

float
CpTf — Free-stream enthalpy.

float
Ts — Sutherland temperature. This is a dimensional unit. Default value is 110.4 K.

float
c1 — Sutherland constant. This is a dimensional unit. Default value is $1.458\times 10^{-6}$ .

float

If muref is not provided, the reference viscosity is computed using the following formula:

$\mu_{\infty} = \frac{C_1 T_{\infty}^{3/2}}{T_{\infty} + T_s}$

Example:

[solver-viscosity-sutherland]
muref = mu
Tref = 300
CpTf = 1 / (gamma -1)*pf/rhof
Ts = 110.4
c1 = 1.458e-6

[solver-time-integrator]

Time integration (or relaxation) schemes and related parameters are configured.

mode — steady or unsteady computation. Currently, dual-time stepping approach is not supported.

steady | unsteady
controller — method to calculate time step size for unsteady simulation.

cfl | dt
cfl — Courant - Friedrichs - Lewy Number. For unsteady simulation, it is required only for cfl controller. For steady simulation, it is a mandatory to solve.

float
dt — time step size for unsteady simulation with dt controller

float
stepper — method to advance time step. For unsteady simulation, there are following options

eulerexplicit | tvd-rk3

For steady simulation, following options can be selected.
eulerexplicit | tvd-rk3 | rk5 | lu-sgs | colored-lu-sgs | jacobi | blu-sgs | colored-blu-sgs
- lu-sgs, blu-sgs — These schemes work only if disabling multi-threading layer (single).
time — initial and the last time for unsteady simulation

float, float
max-iter — the maximum iteration number for steady simulation

int
tolerance — stopping criteria for the magnitude of residual for steady simulation.

float
res-var — the residual variable to apply tolerance stopping criteria. The variable should be selected among the conservative variables. Default variable is rho.

string
coloring — the coloring strategy for colored LU-SGS scheme provided in networkx.greedy_color algorithm. Default variable is largest_first.

string
turb-cfl-factor — The factor of the cfl number for turbulent equations with respect to that of flow equations. It adjusts the pseudo time for turbulence equations to alleviate numerical difficulties. The default value is 1.0.
sub-iter — The maximum iteration number for Jacobi sub-iteration process. The default value is 10.

int
sub-tol — The stopping criteria for the Jacobi sub-iteration. The default value is 0.005.

float
visflux-jacobian — The computing type of viscous Jacobian matrix for several implicit methods.

tlns | approximate | none
- tlns — Based on Thin Layer Navier-Stokes equation (TLNS). Default.
- approximate — Based on Spectral radius. This type computes diagonal elements only.
- none — No viscous flux Jacobian imported. This type can cause convergence delay.
- Applicable methods — jacobi, blu-sgs, colored-blu-sgs

Example for unsteady simulation:

[solver-time-integrator]
controller = cfl
stepper = tvd-rk3
time = 0, 0.25
cfl = 0.9

Example for steady simulation:

[solver-time-integrator]
mode = steady
cfl = 5.0
stepper = colored-lu-sgs
max-iter = 10000
tolerance = 1e-12
res-var = rhou

[solver-cfl-ramp]

If this section is configured, CFL number can be ramped up linearly. Initially CFL number starts from the assigned cfl in [solver-time-integrator].

iter0 — iteration until maintaining the initial CFL.

int
max-iter — final iteration to finish CFL ramping.

int
max-cfl — final CFL

float

Example:

[solver-cfl-ramp]
iter0 = 500
max-iter = 2500
max-cfl = 10.0

Initial and Boundary Conditions

Following sections configure initial and boundary conditions. The position variables (x, y, z) and few numerical functions ( $\sin, \cos, \tanh, \exp, \sqrt {}$ ) and constant ( $\pi$ ) can be used.

Non-dimensionlization

pyBaram does not non-dimensionalize the governing equations, so it is recommended to assign scaled variables for initial and boundary conditions.

The following approach is recommended:

$\rho^* = \frac{\rho}{\rho_{\infty}}, u^* = \frac{u}{a_{\infty}}, p^*=\frac{p}{\rho_{\infty} a_{\infty}^2}, h^*=\frac{h}{a_{\infty}^2}$

Here, $\rho$ , $u$ , and $p$ denote the density, velocity, and pressure, respectively. $a$ denotes the speed of sound, and $h$ denotes the specific enthalpy.

For the free-stream, the non-dimensionalized values can be written as follows:

$\rho^*_{\infty}=1, u^*_{\infty}=M_{\infty}, p^*_{\infty}=\frac{1}{\gamma}, h^*_{\infty}=\frac{1}{\gamma-1}.$

The normalized free-stream viscosity $\mu_{\infty}^*$ is chosen to satisfy Reynolds number $Re_L$ based on the characteristic length $L$ .

$Re_L = \frac{\rho_{\infty} u_{\infty} L}{\mu_{\infty}} = \frac{\rho^*_{\infty} u^*_{\infty} L^*}{\mu^*_{\infty}} \\ \mu_{\infty}^* = \frac{M_{\infty}}{Re_L} L^*$

where $M_{\infty}$ denotes free-stream Mach number. $L^*$ is the non-dimnensionalized characteristic length (i.e., the chord length in the mesh.)

The the viscosity can be calulated via Sutherland law as:

$\mu^* = \mu_{\infty}^* (T^*)^{3/2} \frac{1+T_s / T_{\infty}}{T^* + T_s / T_{\infty}}.$

Here the unit of $T_s, T_{\infty}$ is in Kelvin.

[soln-ics]

The intial condition is configured. All primitive variables should be configured.

Examples:

[soln-ics]
rho = rhof
u = uf*cos(aoa/180*pi)
v = uf*sin(aoa/180*pi)
p = pf

In this, examples, rhof, uf, pf and aoa are assigned at [constants] section.

[soln-bcs-name]

The boundary conditions for the label name is configured. The label should be same as the mesh file (.pbrm).

type — type of boundary condition. To solve Euler system, following types can be used.

slip-wall | sup-out | sup-in | sub-outp | far

To solve Navier-Stokes or RANS system, following types can be used.

slip-wall | adia-wall | isotherm-wall | sup-out | sup-in | sub-outp | sub-inv | far

The details of type and required variables are summarized as follows.

slip-wall — slip wall boundary condition.
adia-wall — adiabatic wall boundary condition.
isotherm-wall — isothermal wall boundary condition.
- CpTw — wall enthalpy
sup-out — supersonic outlet boundary condition
sup-in — supersonic inlet boundary condition
- all primitive variables
sub-outp — subsonic outlet boundary condition with back pressure
- p — back pressure
sub-inv — subsonic inlet boundary condition with velocity
- rho — density
- u, v, w — velocity components.
- turbulent variables
sub-inptt — subsonic inlet boundary condition with total conditions
- p0 — total pressure
- CpT0 — total enthalpy
- dir — velocity direction components.
- turbulent variables
far — far boundary condition
- all primitive variables

Examples:

[soln-bcs-far]
type = far
rho = rhof
u = uf*cos(aoa/180*pi)
v = uf*sin(aoa/180*pi)
p = pf

[soln-bcs-airfoil]
type = adia-wall

Plugins

Plugins in pyBaram serve as post-processing modules after iterations. If a plugin is not configured, no post-processing will occur. The following plugins can be configured:

[soln-plugin-stats]

The stats plugin writes a fundamental log file. For unsteady simulations, it includes time and time step information for each iteration. In steady simulations, it records the residuals of all conservative variables.

flushsteps — flush to file for every flushstep. Default value is 500.

Examples:

[soln-plugin-stats]
flushstep = 300

[soln-plugin-writer]

This plugin writes the solution file.

name — file name. In the name, {n} replaces iteration number and {t} replaces time.
iter-out — write solution file for every iter-out.

Examples:

[soln-plugin-writer]
name = out-{n}
iter-out = 5000

[soln-plugin-force-name]

This plugin computes aerodynamic force and moment coefficients along surface labelled name.

iter-out — compute forces for every iter-out for steady simulation

int
dt-out — compute forces for every dt-out for unsteady simulation

float
rho — reference density to compute dynamic pressure

float
vel — reference velocity to compute dynamic pressure

float
p — reference pressure which is subtracted from the absolute pressure. The relative pressure is integrated along the surface. The default value is zero.

float
area — reference area to compute aerodynamic coefficients

float
length — reference length to compute aerodynamic coefficients

float
force-dir-name — each character (subscript) denote force direction and its direction will be configured.

characters
force-dir- character — component of force direction vector of each subscript character. The dimension of this vector should same as the dimension of space.

float, float, ( float )
moment-center — reference position to compute aerodynamic moment.

float, float, ( float )
moment-dir-name — each character (subscript) denote moment direction and its direction will be configured.

characters
moment-dir- character — component of moment direction vector of each subscript character. For two-dimensional computation, it is a scalar to indicate whether it is clockwise (-1) or counterclockwise (1). For three-dimensional computation, this vector should have the same dimension as the space.

float, float, float

Examples:

[soln-plugin-force-airfoil]
iter-out = 50
rho = rhof
vel = uf
p = pf
area = 1.0
length = 1.0
force-dir-name = ld
force-dir-l = -sin(aoa/180*pi), cos(aoa/180*pi)
force-dir-d = cos(aoa/180*pi), sin(aoa/180*pi)
moment-center = 0.25, 0
moment-dir-name = z
moment-dir-z = -1

[soln-plugin-surface-name]

This plugin integrates variables along the surface labeled as name. It provides both integrated and averaged values.

iter-out — compute forces for every iter-out for steady simulation

int
dt-out — compute forces for every dt-out for unsteady simulation

float
items — items to integrate. Each item is separated by comma

strings
item — expression of item. As well as reserved variables for initial and boundary conditions, nx, ny, nz, which denote the component normal vector, can be used to express item.

Examples:

[soln-plugin-surface-pout]
iter-out = 500
items = p0, mdot
p0 = p*(1+ (gamma-1)/2*(u**2 + v**2)/(gamma*p/rho))**(gamma/(gamma-1))
mdot = rho*(u*nx+v*ny)

In this example, total pressure ( $p_0$ ) and mass flow rate ( $\dot{m}$ ) is computed.

API

pyBaram provides an API for handling I/O and conducting simulations. Currently, only CLI (command line interface) functions are implemented. The basic usage is described as follows:

pybaram.api.io.export_soln(mesh, soln, out)[source]

Export solution to visualization file

Parameters:

mesh (string) – pyBaram mesh file
soln (string) – pyBaram solution file
out (string) – exported file for visualization

pybaram.api.io.import_mesh(inmesh, outmesh, scale=1.0)[source]

Import genreated mesh to pyBaram.

Parameters:

inmesh (string) – Original mesh from generator (CGNS, Gmsh)
outmesh (string) – Converted pyBaram mesh (.pbrm)
scale (float) – Geometric scale factor

pybaram.api.io.partition_mesh(inmesh, outmesh, npart)[source]

Paritioning pyBarm mesh

Parameters:

inmesh (string) – path and name of unspliited pyBaram mesh
outmesh (string) – path and name of patitioned mesh
npart (int) – number of partition

pybaram.api.simulation.restart(mesh, soln, cfg, be='none', comm='none')[source]

Restarted run from mesh and configuration files.

Parameters:

mesh (pyBaram mesh) – pyBaram NativeReader object
soln (pyBaram solution) – pyBaram NativeReader object
cfg (config) – pyBaram INIFile object
be (Backend) – pyBaram backend object
comm (MPI communicator) – mpi4py comm object

pybaram.api.simulation.run(mesh, cfg, be='none', comm='none')[source]

Fresh run from mesh and configuration files.

Parameters:

mesh (pyBaram mesh) – pyBaram NativeReader object
cfg (config) – pyBaram INIFile object
be (Backend) – pyBaram backend object
comm (MPI communicator) – mpi4py comm object