Session file configuration

9.3 Session file configuration

In the following we describe the session file configuration. Specifically we consider the sections under the tag <CONDITIONS> in the session (.xml) file.

Parameters

Under this section it is possible to set the parameters of the simulation.

1<PARAMETERS> 
2  <P> TimeStep            = 0.0000001                  </P> 
3  <P> FinTime             = 1.0                        </P> 
4  <P> NumSteps            = FinTime/TimeStep           </P> 
5  <P> IO_CheckSteps       = 5000                       </P> 
6  <P> IO_InfoSteps        = 1                          </P> 
7  <P> Gamma               = 1.4                        </P> 
8  <P> pInf                = 101325                     </P> 
9  <P> rhoInf              = 1.225                      </P> 
10  <P> GasConstant         = 287.058                    </P> 
11  <P> TInf                = pInf/(287.058*rhoInf)      </P> 
12  <P> Twall               = pInf/(287.058*rhoInf)+15.0 </P> 
13  <P> uInf                = 147.4                      </P> 
14  <P> vInf                = 0.0                        </P> 
15  <P> wInf                = 0.0                        </P> 
16  <P> mu                  = 1e-5                       </P> 
17  <P> Pr                  = 0.72                       </P> 
18  <P> thermalConductivity = 0.02                       </P> 
19  <P> IO_Timer_Level      = 3                          </P> 
20</PARAMETERS>

TimeStep is the time-step we want to use.
FinTime is the final physical time at which we want our simulation to stop.
NumSteps is the equivalent of FinTime but instead of specifying the physical final time we specify the number of time-steps.
IO_CheckSteps sets the number of steps between successive checkpoint files. No checkpoint file is written if it is set to 0.
IO_InfoSteps sets the number of steps between successive info stats are printed to screen.
Gamma ratio of the specific heats. Default value = 1.4.
pInf farfield pressure (i.e. p_∞). Default value = 101325 Pa.
rhoInf farfield density (i.e. ρ_∞). Default value = 1.225 Kg∕m³.
GasConstant universal gas contant. Default value = 287.058 JKg^-1K^-1.
TInf farfield temperature (i.e. T_∞). Default value = 288.15 K.
Twall temperature at the wall when isothermal boundary conditions are employed (i.e. T_w). Default value = 300.15K.
uInf farfield X-component of the velocity (i.e. u_∞). Default value = 0.1 m∕s.
vInf farfield Y -component of the velocity (i.e. v_∞). Default value = 0.0 m∕s.
wInf farfield Z-component of the velocity (i.e. w_∞). Default value = 0.0 m∕s.
mu dynamic viscosity (i.e. μ_∞). Default value = 1.78e-05 Pas.
Pr Prandtl number. Default value = 0.72.
thermalConductivity thermal conductivity (i.e. κ_∞). This can be set as an alternative to Pr, in which case the Prandtl number is calculated from κ_∞ (it is only possible to set one of them). By default, this is obtained from the Prandtl number.
CFL is the CFL number (explicit and implicit solvers).
CFLGrowth is the growing CFL (explicit and implicit solvers).
CFLEnd is the maximum value of the CFL number (explicit and implicit solvers).
Timer_IO_Level defines the amount of timer information that is printed after the solver is finished. The default value is -1, which disables output. By selecting a value between 0 and 2, more detailed timer information is printed.

Time Integration Scheme

Under this section it is possible to set the time integration scheme information.

1<TIMEINTEGRATIONSCHEME> 
2  <METHOD> RungeKutta </METHOD> 
3  <VARIANT> SSP </VARIANT> 
4  <ORDER> 3 </ORDER> 
5</TIMEINTEGRATIONSCHEME>

TimeIntegrationScheme is the time-integration scheme we want to use. There are implicit and explicit schemes for the Compressible flow solver. For an explicit discretization, the time-integration schemes supported are as follows

Name	<METHOD>	<VARIANT>	<ORDER>
Forward Euler	ForwardEuler	-	1
Runge Kutta 2 - SSP	RungeKutta	SSP	2
Runge Kutta 3 - SSP	RungeKutta	SSP	3
Runge Kutta 4	ClassicalRungeKutta	-	4
Runge Kutta 5	RungeKutta	-	5

For an implicit discretization, the time-integration schemes available are

Name	<METHOD>	<VARIANT>	<ORDER>
Backward Euler	BackwardEuler	-	1
Backward Differentiation Formula Implicit	BDFImplicit	-	1
Backward Differentiation Formula Implicit	BDFImplicit	-	2
Singly Diagonally Implicit Runge Kutta	DIRK	-	2
Singly Diagonally Implicit Runge Kutta	DIRK	-	3
Singly Diagonally Implicit Runge Kutta	DIRK	ES5	3
Singly Diagonally Implicit Runge Kutta	DIRK	-	4
Singly Diagonally Implicit Runge Kutta	DIRK	ES5	4

Solver info

Under this section it is possible to set the solver information.

1<SOLVERINFO> 
2  <I PROPERTY="EQTYPE"                        VALUE="NavierStokesImplicitCFE" /> 
3  <I PROPERTY="Projection"                    VALUE="DisContinuous"           /> 
4  <I PROPERTY="TimeIntegrationMethod"         VALUE="DIRKOrder2"              /> 
5  <I PROPERTY="AdvectioType"                  VALUE="WeakDG"                  /> 
6  <I PROPERTY="DiffusionType"                 VALUE="InteriorPenalty"         /> 
7  <I PROPERTY="UpwindType"                    VALUE="Roe"                     /> 
8  <I PROPERTY="ProblemType"                   VALUE="General"                 /> 
9  <I PROPERTY="ViscosityType"                 VALUE="Constant"                /> 
10  <I PROPERTY="EquationOfState"               VALUE="IdealGas"                /> 
11  <I PROPERTY="Driver"                        VALUE="Standard"                /> 
12</SOLVERINFO>

EQType is the tag which specify the equations we want solve:

Explicit discretization in time:
- NavierStokesCFE (Compressible Navier-Stokes equations).
- EulerCFE (Compressible Euler equations).
Implicit discretization in time:
- NavierStokesImplicitCFE (Compressible Navier-Stokes equations).
- EulerImplicitCFE (Compressible Euler equations).
Projection is the type of projection we want to use:
- DisContinuous.
  Note that the Continuous projection is not supported in the Compressible Flow Solver.
AdvectionType is the advection operator we want to use.
- WeakDG (classical DG in weak form).
- FRDG (Flux-Reconstruction recovering nodal DG scheme).
- FRSD (Flux-Reconstruction recovering a spectral difference (SD) scheme).
- FRHU (Flux-Reconstruction recovering Huynh (G2) scheme).
- FRcmin (Flux-Reconstruction with c = c_min).
- FRcinf (Flux-Reconstruction with c = ∞).
Note that only WeakDG is fully supported, the other operators work only with quadrilateral elements (2D or 2.5D).
DiffusionType is the diffusion operator we want to use for the Navier-Stokes equations:
- LDGNS (LDG with primitive variables. The penalty term is inversely proportional to the element size, proportional to the local viscosity for the momentum equations and to the thermal conductivity for the energy equation, and proportional to an optional parameter LDGNSc11 which is by default set to one; proportionality to polynomial order can be manually imposed by setting the parameter LDGNSc11 equal to p²).
- LFRDGNS (Flux-Reconstruction recovering nodal DG scheme).
- LFRSDNS (Flux-Reconstruction recovering a spectral difference (SD) scheme).
- LFRHUNS (Flux-Reconstruction recovering Huynh (G2) scheme).
- LFRcminNS (Flux-Reconstruction with c = c_min).
- LFRcinfNS (Flux-Reconstruction with c = ∞).
- InteriorPenalty (Symmetric interior penalty method).
Note that only LDGNS and InteriorPenalty are fully supported, the other operators work only with quadrilateral elements (2D or 2.5D).
UpwindType is the numerical interface flux (i.e. Riemann solver) we want to use for the advection operator:
- AUSM0.
- AUSM1.
- AUSM2.
- AUSM3.
- Average.
- ExactToro.
- HLL.
- HLLC.
- LaxFriedrichs.
- Roe.
ViscosityType is the viscosity type we want to use:
- Constant (Constant viscosity).
- Variable (Variable viscosity through the Sutherland’s law).
EquationOfState allows selecting an equation of state for accounting for non-ideal gas behaviour:
- IdealGas (default option).
- VanDerWaals (requires additional parameters Tcrit and Pcrit).
- RedlichKwong (requires additional parameters Tcrit and Pcrit).
- PengRobinson (requires additional parameters Tcrit, Pcrit and AcentricFactor).
Driver specifies the type of problem to be solved:
- Standard (default option to solve the unsteady equations).
- SteadyState (uses the Selective Frequency Damping method (see Sec. 11.1.4) to obtain a steady-state solution of the Navier-Stokes equations (explicit or implicit)).
ShockCaptureType specifies the type of operator to be used for shock capturing:
- NonSmooth add a Laplacian operator to apply artificial diffusion (see Sec. 9.4.1.1). This option is only supported for explicit solvers (EulerCFE and NavierStokesCFE).
- Physical add artificial viscosity to the physical viscosity. This option is only supported for Navier-Stokes solvers (NavierStokesCFE and NavierStokesImplicitCFE).
ShockSensorType specifies the sensor type of shock capturing to be used:
- Modal (default) use a modal sensor to identify where to add viscosity (see Sec. 9.4.1.2).
- Dilatation use a dilatation sensor to identify where to add viscosity.
DucrosSensor apply a Ducros [12] (anti-vorticity) filter to the shock sensor:
- On
- Off
Smoothing apply a smoothing filter to the shock sensor:
- C0 smooth the artificial viscosity to be a continuous field.

Boundary conditions

In this section we can specify the boundary conditions for our problem. First we need to define the variables under the section VARIABLES. For a 1D problem we have:

1<VARIABLES> 
2  <V ID="0"> rho  </V> 
3  <V ID="1"> rhou </V> 
4  <V ID="2"> E    </V> 
5</VARIABLES>

For a 2D problem we have

1<VARIABLES> 
2  <V ID="0"> rho  </V> 
3  <V ID="1"> rhou </V> 
4  <V ID="2"> rhov </V> 
5  <V ID="3"> E    </V> 
6</VARIABLES>

For a 3D problem we have:

1<VARIABLES> 
2  <V ID="0"> rho  </V> 
3  <V ID="1"> rhou </V> 
4  <V ID="2"> rhov </V> 
5  <V ID="3"> rhow </V> 
6  <V ID="4"> E    </V> 
7</VARIABLES>

After having defined the variables depending on the dimensions of the problem we want to solve, it is necessary to specify the boundary regions on which we want to define the boundary conditions:

1<BOUNDARYREGIONS> 
2  <B ID="0"> C[100] </B> 
3</BOUNDARYREGIONS>

Finally we can specify the boundary conditions on the regions specified under BOUNDARYREGIONS. Note that the no-slip, isothermal, wall boundary condition requires Twall to be specified. In the following are some examples for a 2D problem:

Slip wall boundary conditions:

1<BOUNDARYCONDITIONS> 
2  <REGION REF="0"> 
3    <D VAR="rho"  USERDEFINEDTYPE="Wall" VALUE="0" /> 
4    <D VAR="rhou" USERDEFINEDTYPE="Wall" VALUE="0" /> 
5    <D VAR="rhov" USERDEFINEDTYPE="Wall" VALUE="0" /> 
6    <D VAR="E"    USERDEFINEDTYPE="Wall" VALUE="0" /> 
7  </REGION> 
8</BOUNDARYCONDITIONS>

No-slip wall boundary conditions:

1<BOUNDARYCONDITIONS> 
2  <REGION REF="0"> 
3    <D VAR="rho"  USERDEFINEDTYPE="WallViscous" VALUE="0" /> 
4    <D VAR="rhou" USERDEFINEDTYPE="WallViscous" VALUE="0" /> 
5    <D VAR="rhov" USERDEFINEDTYPE="WallViscous" VALUE="0" /> 
6    <D VAR="E"    USERDEFINEDTYPE="WallViscous" VALUE="0" /> 
7  </REGION> 
8</BOUNDARYCONDITIONS>

Adiabatic wall boundary conditions:

1<BOUNDARYCONDITIONS> 
2  <REGION REF="0"> 
3    <D VAR="rho"  USERDEFINEDTYPE="WallAdiabatic" VALUE="0" /> 
4    <D VAR="rhou" USERDEFINEDTYPE="WallAdiabatic" VALUE="0" /> 
5    <D VAR="rhov" USERDEFINEDTYPE="WallAdiabatic" VALUE="0" /> 
6    <D VAR="E"    USERDEFINEDTYPE="WallAdiabatic" VALUE="0" /> 
7  </REGION> 
8</BOUNDARYCONDITIONS>

In some cases we need to excite perturbations inside the boundary layer. This can be achieved by setting part of the wall as a disturbance strip. In the no-slip/adiabatic wall boundary conditions, if the VALUE is not exact "0" but any expression, which can be time-dependent, the value of the expression will be added to the ghost state of what it should be in the input boundary conditions, and then generate a non-zero flux through the Riemann solver. The following is an example to set a disturbance strip of amplitude A, frequency f, and in the range of [x₀,x₀ + len] on a flat plate.

1  <BOUNDARYCONDITIONS> 
2    <REGION REF="0"> 
3      <D VAR="rho"  USERDEFINEDTYPE="WallAdiabatic" VALUE="0" /> 
4      <D VAR="rhou" USERDEFINEDTYPE="WallAdiabatic" VALUE="0" /> 
5      <D VAR="rhov" USERDEFINEDTYPE="WallAdiabatic" 
6                    VALUE="A*sin(2*PI*f*t)*sin(2*PI*(x-x0)/len) 
7                            *(x>=x0)*(x<=(x0+len))"           /> 
8      <D VAR="E"    USERDEFINEDTYPE="WallAdiabatic" VALUE="0" /> 
9    </REGION> 
10  </BOUNDARYCONDITIONS>

Farfield boundary conditions (including inviscid characteristic boundary conditions):

1<BOUNDARYCONDITIONS> 
2  <REGION REF="0"> 
3    <D VAR="rho"  VALUE="rhoInf" /> 
4    <D VAR="rhou" VALUE="rhoInf*uInf" /> 
5    <D VAR="rhov" VALUE="rhoInf*vInf" /> 
6    <D VAR="E" 
7    VALUE="pInf/(Gamma-1)+0.5*rhoInf*(uInf*uInf+vInf*vInf)"/> 
8  </REGION> 
9</BOUNDARYCONDITIONS>

Pressure outflow boundary conditions:

1<BOUNDARYCONDITIONS> 
2  <REGION REF="0"> 
3    <D VAR="rho"  USERDEFINEDTYPE="PressureOutflow" VALUE="0" /> 
4    <D VAR="rhou" USERDEFINEDTYPE="PressureOutflow" VALUE="0" /> 
5    <D VAR="rhov" USERDEFINEDTYPE="PressureOutflow" VALUE="0" /> 
6    <D VAR="E"    USERDEFINEDTYPE="PressureOutflow" VALUE="pOut" /> 
7  </REGION> 
8</BOUNDARYCONDITIONS>

where pOut is the target static pressure at the boundary.

Stagnation inflow boundary condition:
```
1<BOUNDARYCONDITIONS> 
2  <REGION REF="0"> 
3    <D VAR="rho"  USERDEFINEDTYPE="StagnationInflow" VALUE="rho0" /> 
4    <D VAR="rhou" USERDEFINEDTYPE="StagnationInflow" VALUE="nx" /> 
5    <D VAR="rhov" USERDEFINEDTYPE="StagnationInflow" VALUE="ny" /> 
6    <D VAR="rhov" USERDEFINEDTYPE="StagnationInflow" VALUE="nz" /> 
7    <D VAR="E"    USERDEFINEDTYPE="StagnationInflow" VALUE="p0/(Gamma-1)" /> 
8  </REGION> 
9</BOUNDARYCONDITIONS>
```
where rho0 and p0 are the stagnation density and stagnation pressure, respectively. The values nx, ny, and nz further define the direction of the flow. Note that it is not necessary to normalize the vector (nx, ny, nz), it will be done automatically by the solver. If the flow direction isn’t specified, the flow will enter in the boundary-normal direction. The stagnation inflow boundary condition imposes a constant stagnation density and stagnation pressure on the boundary. These quantities are related to the stagnation temperature through the relation T0 = p0/(rho0 * GasConstant). This boundary condition is useful in situations when stagnation quantities are known at the inlet, rather than the actual density and pressure. In addition to this, the standard boundary condition where 5 quantities (the conservative variables) are imposed on the boundary is not suitable in many situations because in a subsonic compressible flow, only 4 out of 5 variables can be imposed at an inlet boundary. In contrast, the stagnation inflow boundary condition only imposes 4 quantities (2 stagnation quantities, and the direction of the flow). The last quantitity at the inlet will instead be determined by the solution inside the domain. If you have a good estimate of one additional quantitity at the inlet, such as the magnitude of the velocity or the static pressure, you can estimate all remaining quantities at the inlet for the isentropic compressible flow relations. In fact, at each iteration, the solver uses the isentropic flow relations combined with the quantities imposed by the boundary + one quantity from the interior solution to compute all remaining quantities at the boundary. Once this has been done, the flux over the boundary at that iteration can be computed.

Subsonic boundary condition enforcing entropy and pressure:

1<BOUNDARYCONDITIONS> 
2  <REGION REF="0"> 
3    <D VAR="rho"  USERDEFINEDTYPE="EnforceEntropyPressure" VALUE="rhoInf" /> 
4    <D VAR="rhou" USERDEFINEDTYPE="EnforceEntropyPressure" VALUE="rhoInf*uInf" /> 
5    <D VAR="rhov" USERDEFINEDTYPE="EnforceEntropyPressure" VALUE="rhoInf*vInf" /> 
6    <D VAR="rhov" USERDEFINEDTYPE="EnforceEntropyPressure" VALUE="rhoInf*wInf" /> 
7    <D VAR="E"    USERDEFINEDTYPE="EnforceEntropyPressure" VALUE="pInf/(Gamma-1) + 0.5*rhoInf*(uInf*uInf + vInf*vInf)" /> 
8  </REGION> 
9</BOUNDARYCONDITIONS>

where the input type can be either VALUE or FILE such that the specified entropy and pressure distribution (corresponding to the input rhoInf, rhoInf*uInf, rhoInf*vInf, rhoInf*wInf, and E) will be enforced on the subsonic inflow boundary. If the flow is supersonic, all the conditions are naturelly agreed with the input distribution. The following two conditions follows the same rule.

Subsonic boundary condition enforcing entropy and velocity:

1<BOUNDARYCONDITIONS> 
2  <REGION REF="0"> 
3    <D VAR="rho"  USERDEFINEDTYPE="EnforceEntropyVelocity" VALUE="rhoInf" /> 
4    <D VAR="rhou" USERDEFINEDTYPE="EnforceEntropyVelocity" VALUE="rhoInf*uInf" /> 
5    <D VAR="rhov" USERDEFINEDTYPE="EnforceEntropyVelocity" VALUE="rhoInf*vInf" /> 
6    <D VAR="rhov" USERDEFINEDTYPE="EnforceEntropyVelocity" VALUE="rhoInf*wInf" /> 
7    <D VAR="E"    USERDEFINEDTYPE="EnforceEntropyVelocity" VALUE="pInf/(Gamma-1) + 0.5*rhoInf*(uInf*uInf + vInf*vInf)" /> 
8  </REGION> 
9</BOUNDARYCONDITIONS>

where both tangential and normal velocity components are enforced. Therefore the angle of attack is maintained.

Subsonic boundary condition enforcing entropy and total enthalpy:

1<BOUNDARYCONDITIONS> 
2  <REGION REF="0"> 
3    <D VAR="rho"  USERDEFINEDTYPE="EnforceEntropyTotalEnthalpy" VALUE="rhoInf" /> 
4    <D VAR="rhou" USERDEFINEDTYPE="EnforceEntropyTotalEnthalpy" VALUE="rhoInf*uInf" /> 
5    <D VAR="rhov" USERDEFINEDTYPE="EnforceEntropyTotalEnthalpy" VALUE="rhoInf*vInf" /> 
6    <D VAR="rhov" USERDEFINEDTYPE="EnforceEntropyTotalEnthalpy" VALUE="rhoInf*wInf" /> 
7    <D VAR="E"    USERDEFINEDTYPE="EnforceEntropyTotalEnthalpy" VALUE="pInf/(Gamma-1) + 0.5*rhoInf*(uInf*uInf + vInf*vInf)" /> 
8  </REGION> 
9</BOUNDARYCONDITIONS>

Initial conditions and exact solution

Under the two following sections it is possible to define the initial conditions and the exact solution (if existent).

1<FUNCTION NAME="InitialConditions"> 
2  <E VAR="rho"    VALUE="rhoInf"/> 
3  <E VAR="rhou"   VALUE="rhoInf*uInf"   /> 
4  <E VAR="rhov"   VALUE="rhoInf*vInf"   /> 
5  <E VAR="E" 
6  VALUE="pInf/(Gamma-1)+0.5*rhoInf*(uInf*uInf+vInf*vInf)"/> 
7</FUNCTION> 
8 
9<FUNCTION NAME="ExactSolution"> 
10  <E VAR="rho"    VALUE="rhoInf"          /> 
11  <E VAR="rhou"   VALUE="rhoInf*uInf"   /> 
12  <E VAR="rhov"   VALUE="rhoInf*vInf"   /> 
13  <E VAR="E" 
14  VALUE="pInf/(Gamma-1)+0.5*rhoInf*(uInf*uInf+vInf*vInf)"/> 
15</FUNCTION>

[next] [prev] [prev-tail] [front] [up]