Skip to content

Latest commit

 

History

History
331 lines (260 loc) · 20.7 KB

Solver-Setup.md

File metadata and controls

331 lines (260 loc) · 20.7 KB
title permalink
Solver Setup
/docs_v7/Solver-Setup/

This is a basic introduction on how to set up a simulation using SU2. We distinguish between single-zone computations and multi-zone computations. The following considers a single zone only. For an explanation on multi-zone problems, continue with Basics of Multi-Zone Computations.

Three different types of mathematical problem can be solved in SU2. The type is specified via the MATH_PROBLEM config option. The options are: DIRECT: Also referred to as primal, this is the default when SU2_CFD or SU2_DEF are used. DISCRETE_ADJOINT: A discrete adjoint methodology based on Automatic Differentiation, available for most solvers. This is the default for SU2_CFD_AD and SU2_DOT_AD CONTINUOUS_ADJOINT: A hand-derived continuous adjoint methodology available only for compressible flows.

See the Software Components documentation to determine which software module is required for each problem.

Defining the Problem

Solver Version
ALL 7.3.1

Direct

SU2 is capable of dealing with different kinds of physical problems. The kind of problem is defined by choosing a solver using the SOLVER option. The list of possible values and a description can be found in the following table:

Option Value Problem Type
EULER Euler's equation Finite-Volume method
NAVIER_STOKES Navier-Stokes' equation Finite-Volume method
RANS Reynolds-averaged Navier-Stokes' equation Finite-Volume method
INC_EULER Incompressible Euler's equation Finite-Volume method
INC_NAVIER_STOKES Incompressible Navier-Stokes' equation Finite-Volume method
INC_RANS Incompressible Reynolds-averaged Navier-Stokes' equation Finite-Volume method
HEAT_EQUATION_FVM Heat equation Finite-Volume method
ELASTICITY Equations of elasticity Finite-Element method
FEM_EULER Euler's equation Discontinuous Galerkin FEM
FEM_NAVIER_STOKES Navier-Stokes' equation Discontinuous Galerkin FEM
MULTIPHYSICS Multi-zone problem with different solvers in each zone -

Turbulence modeling

This section describes how to define the turbulence model in SU2 to be coupled to RANS or INC_RANS. The selected model must be specified in the config file by the KIND_TURB_MODEL option. The current available turbulence models are the:

  • NONE: No turbulence model.
  • SST: Mentor Shear Stress Transport.
  • SA: Spalart-Allmaras.

Different corrections and variations are implemented for each turbulence model. These are specified accordingly either in SST_OPTIONS or in SA_OPTIONS. The folowing options are available:

  • SST_OPTIONS:

    • NONE: No SST turbulence model (default).
    • V1994m: refers to the "Standard" Menter SST model from 1994 with the modified constant $\sigma_{k1}$ and the redefinition of the turbulent eddy viscosity.
    • V2003m: refers to the Menter SST model from 2003 ignoring the $\tau_{ij}$ in the momentum and energy equations and the production term is approximated by $P = \mu_t S^2$.
    • VORTICITY: refers to the vorticity source term correction.
    • KATO_LAUNDER: refers to the Kato-Launder correction.
    • UQ: refers to the V1994m version with uncertainty quantification modifications.??
    • SUSTAINING: refers to the controlled decay correction.

  • SA_OPTIONS:

    • NONE: refers to the modification where the $f_{t2}$ term is set to zero, i.e., $c_{t3} = 0$ (default).
    • NEGATIVE: refers to the negative Spalart-Allmaras modification.
    • EDWARDS: refers to the so-called Edwards modification.
    • WITHFT2: refers to the standalone version.
    • QCR2000: refers to the Quadratic Constitutive Relation modification, 2000 version.
    • COMPRESSIBILITY: refers to the Mixing Layer Compressibility modification.
    • ROTATION: refers to the rotation and curvature effects correction.
    • BCM: refers to the SA-BCM transitional turbulence model.
    • EXPERIMENTAL: Allow experimental combinations of options (according to NASA TMR).

We refer for example to NASA TMR for a detailed explanation and definition of each correction and variation.

Spalart-Allamaras

The single transported Spalart-Allmaras variable $\tilde{\nu}$ is initialized with the value at the farfield or inlet boundary. As suggested in the literature, the value there is computed as $\tilde{\nu}/\nu=\text{turb2lam}$. In SU2 the free-stream Spalart-Allmaras variable to kinematic laminar viscosity ratio, $\text{turb2lam}$, is defined by the FREESTREAM_NU_FACTOR config file field. The default value is $\tilde{\nu}/\nu = 3.0$ avoiding laminar solutions.

An extension of SU2 includes an hybrid turbulence model: the Spalart-Allmaras original model with Detached-Eddy Simulation (DES) modification. Refer to Eduardo Moina's thesis?. The use of the hybrid RANS/LES model is specified in the cofig file with the field HYBRID_RANSLES. Four different techniques are currently implemented:

  • SA_DES Detached-Eddy Simulation
  • SA_DDES Delayed Detached-Eddy Simulation
  • SA_ZDES Zonal Detached-Eddy Simulation
  • SA_EDDES Enhanced Detached-Eddy Simulation

The DES constant can be controlledd by the field DES_CONST, with 0.65 as default.

Menter’s k-omega SST Model

As initial conditions, the values of are initialized at all grid point with the farfield values. The farfield conditions for the turbulent kinetic energy $k$ is computed as: $k = \frac{3}{2}(UI)$, whereby $U$ is the freestream velocity magnitude and $I$ is the turbulence intensity. This latter value can be specified in the config file by the FREESTREAM_TURBULENCEINTENSITY field, with defaul value to 0.05 which corresponds to a $5%$. The freestream value of the turbulent frequency $\omega$ is computed as: $\omega = \frac{\rho k}{\mu}(\frac{\mu_t}{\mu})^{-1}$, where $\rho$ and $\mu$ are the freestream density and laminar viscosity respectively and $\frac{\mu_t}{\mu}$ is the turbulent viscosity ratio, also known as freestream dissipation. Its value can be specified in the FREESTREAM_TURB2LAMVISCRATIO field, defaulting to $10$.

Limitations of k and omega

To increase robustness and prevent negative values, a hard-coded upper and lower limit are set for each turbulent variable:

// turbulence kinetic energy
lowerlimit = 1.0e-10;
upperlimit = 1.0e10;

// 
lowerlimit = 1.0e-4;
upperlimit = 1.0e15;

Further, by the model definition in the farfield region there is no production of $k$ nor $\omega$ while destruction still takes place. Consequently the turbulence quantities typically decay on their way from the farfield boundary to the airfoil. In order to prevent the non-physical decay in SU2 there are implemented to two approaches:

  • Sustaining terms: it consists on the introduction of additional source terms in the turbulence model equations compensating the destruction terms in the farfield flow. This approach is activated by using the modified version of the SST moodel, SST-sust.
  • Floor values: this approach is equivalent to setting the lowerlimit to the farfield values in the upstream region of an airfoil. The floor values are implemented in the form of fixed values. This correction can be activated with the following parameters in the config file: TURB_FIXED_VALUES= YES TURB_FIXED_VALUES_DOMAIN= -1.0 To determine those grid points where the correction should be applied, we compare the dot product of the normalized freestream velocity vector and the grid point coordinates. For those points which dot product result is lower than the specified TURB_FIXED_VALUES_DOMAIN value, the turbulence quantities are just set to the farfield values there. Note that although the Spalart-Allmaras turbulence model does not suffer from a decaying turbulence variable, the floor values limitation can also be employed.

Foward mode of AD

The forward mode of AD capability allows to compute the forward derivatives (see Advanced AD Techniques) of an specified function with respect to a registered variable/s. If multiple design variables are registered as input, the output will consist on the accumulation. The function to be differentiated can be any of the variables specified as COEFFICIENT in the SetHistoryOutputFields functions of the flow output classes. To get the derivative, one just needs to write D_< string group name > in the HISTORY_OUTPUT field from the config file. Addioiniallty, the field DIRECT_DIFF specifies the variable to be registered as an input. In SU2 it is possible to register almost any variable. Currently SU2 has implemented the following variables:

D_MACH Freestream Mach number D_AOA angle of attack D_PRESSURE freestream pressure D_TEMPERATURE freestream temperature D_DENSITY freestream density D_TURB2LAM freestream ratio of turbulent to laminar viscosity D_SIDESLIP sideslip angle D_VISCOSITY freestream laminar viscosity D_REYNOLDS freestream Reynolds number D_DESIGN design?? D_YOUNG Young's modulus D_POISSON Poisson's ratio D_RHO solid density (inertial) D_RHO_DL density for dead loads D_EFIELD electric field

The execution of this capability is done by the module SU2_CFD_DIRECTDIFF. See the Software Components for further details.

Adjoint Formulations

Discrete adjoint

SU2 can compute the sensitivities of an objective function with respect to the control points defining the shape of the design surface. For the detailed list of available objective functions in SU2 we address to the enumeration declaration 'ENUM_OBJECTIVE'. The associated nomenclature for the configuration file is specified in 'Objective_Map'

The objective function value can be scaled by a weighting factor. This value can be specified in the OBJECTIVE_WEIGHT field on the config file.

Continuous adjoint

Same as the discrete adjoint but using the continuous adjoint approach :)

Every solver has its specific options and we refer to the tutorial cases for more information. However, the basic controls detailed in the remainder of this page are the same for all problems.

Restarting the simulation

Solver Version
ALL 7.3.1

A simulation can be restarted from a previous computation by setting RESTART_SOL=YES. The field data is imported from the restart file SOLUTION_FILENAME and must be located in the same directory. The solution file can be either a .csv or .dat file. The number of points must be the same as that for the simulation. If it is a time-dependent problem, additionally RESTART_ITER must be set to the time iteration index you want to restart from. For example, the following code will restart an unsteady problem from iteration number 2:

% ------------------------- Solver definition -------------------------------%
%
% Type of solver 
SOLVER= EULER
%
% Restart solution (NO, YES)
RESTART_SOL= YES
%
% Iteration number to begin unsteady restarts (used if RESTART_SOL= YES)
RESTART_ITER= 2
%

Additionally the solution files solution_flow_00000 and solution_flow_00001, corresponding to steps or iteration 0 and 1 respectively, will be used for restarting the simulation.

Controlling the simulation

Solver Version
ALL 7.3.1

A simulation is controlled by setting the number of iterations the solver should run (or by setting a convergence critera). The picture below depicts the two types of iterations we consider.

Types of Iteration

SU2 makes use of an outer time loop to march through the physical time, and of an inner loop which is usually a pseudo-time iteration or a (quasi-)Newton scheme. The actual method used depends again on the specific type of solver.

Courant-Friedrichs-Lewy number

The Courant-Friedrichs-Lewy number is specified by the CFL_NUMBER parameter. It is possible to adapt locally its magnitude on each pseudo-iteration according to the solver residual convergence. To enable this capability, the CFL_ADAPT must be set to YES.

The option CFL_ADAPT_PARAM controls the adaptative CFL number, which parameters are: factor-down, factor-up, CFL min value, CFL max value and acceptable linear solver convergence.

If an adaptative CFL number is used, the initial CFL number for the finest grid is set to . The local CFL number increases by until if the solution rate of change is not limited, and acceptable linear convergence is achieved. It is reduced by if rate is limited, there is not enough linear convergence, or the nonlinear residuals are stagnant and oscillatory. It is reset back to when linear solvers diverge, or if nonlinear residuals increase too much.

No idea about the acceptable parameter?

Time-dependent Simulation

Solver Version
ALL 7.3.1

To enable a time-dependent simulation set the option TIME_DOMAIN to YES (default is NO). There are different methods available for certain solvers which can be set using the TIME_MARCHING option. For example for any of the FVM-type solvers a first or second-order dual-time stepping (DUAL_TIME_STEPPING-1ST_ORDER/DUAL_TIME_STEPPING-2ND_ORDER) method or a conventional time-stepping method (TIME_STEPPING) can be used.

% ------------------------- Time-dependent Simulation -------------------------------%
%
TIME_DOMAIN= YES
%
% Time Step for dual time stepping simulations (s)
TIME_STEP= 1.0
%
% Total Physical Time for dual time stepping simulations (s)
MAX_TIME= 50.0
%
% Number of internal iterations 
INNER_ITER= 200
%
% Number of time steps
TIME_ITER= 200
%

The solver will stop either when it reaches the maximum time (MAX_TIME) or the maximum number of time steps (TIME_ITER), whichever event occurs first. Depending on the TIME_MARCHING option, the solver might use an inner iteration loop to converge each physical time step. The number of iterations within each time step is controlled using the INNER_ITER option.

Steady-state Simulation

Solver Version
ALL 7.3.1

A steady-state simulation is defined by using TIME_DOMAIN=NO, which is the default value if the option is not present. In this case the number of iterations is controlled by the option ITER.

Note: To make it easier to switch between steady-state, time-dependent and multizone simulations, the option INNER_ITER can also be used to specify the number of iterations. If both options are present, INNER_ITER has precedence.

Setting convergence criteria

Solver Version
ALL 7.3.1

Despite setting the maximum number of iterations, it is possible to use a convergence criterion so that the solver will stop when it reaches a certain value of a residual or if variations of a coefficient are below a certain threshold. To enable a convergence criterion use the option CONV_FIELD to set an output field that should be monitored. The list of possible fields depends on the solver. Take a look at Custom Output to learn more about output fields. Depending on the type of field (residual or coefficient) there are two types of methods:

Steady-state Residual

If the field set with CONV_FIELD is a residual, the solver will stop if it is smaller than the value set with CONV_RESIDUAL_MINVAL option. Example:

% ------------------- Residual-based Convergence Criteria -------------------------%
%
CONV_FIELD= RMS_DENSITY
%
%
% Min value of the residual (log10 of the residual)
CONV_RESIDUAL_MINVAL= -8
%

Steady-state Coefficient

If the field set with CONV_FIELD is a coefficient, a Cauchy series approach is applied. A Cauchy element is defined as the relative difference of the coefficient between two consecutive iterations. The solver will stop if the average over a certain number of elements (set with CONV_CAUCHY_ELEMS) is smaller than the value set with CONV_CAUCHY_EPS. The current value of the Cauchy coefficient can be written to screen or history by adding the CAUCHY field to the SCREEN_OUTPUT or HISTORY_OUTPUT option (see Custom Output). Example:

% ------------------ Coefficient-based Convergence Criteria -----------------------%
%
CONV_FIELD= DRAG
%
%
% Number of elements to apply the criteria
CONV_CAUCHY_ELEMS= 100
%
% Epsilon to control the series convergence
CONV_CAUCHY_EPS= 1E-10
%

For both methods the option CONV_STARTITER defines when the solver should start monitoring the criterion.

Time-dependent Coefficient

In a time-dependend simulation we have two iterators, INNER_ITER and TIME_ITER. The convergence criterion for the INNER_ITER loop is the same as in the steady-state case. For the TIME_ITER, there are convergence options implemented for the case of a periodic flow. The convergence criterion uses the so-called windowing approach, (see Custom Output). The convergence options are applicable only for coefficients. To enable time convergence, set WINDOW_CAUCHY_CRIT=YES (default is NO). The option CONV_WINDOW_FIELD determines the output-fields to be monitored. Typically, one is interested in monitoring time-averaged coefficients, e.g TAVG_DRAG. Analogously to the steady state case, the solver will stop, if the average over a certain number of elements (set with CONV_WINDOW_CAUCHY_ELEMS) is smaller than the value set with CONV_WINDOW_CAUCHY_EPS. The current value of the Cauchy coefficient can be written to screen or history using the flag CAUCHY (see Custom Output). The option CONV_WINDOW_STARTITER determines the numer of iterations, the solver should wait to start moniotring, after WINDOW_START_ITER has passed. WINDOW_START_ITER determines the iteration, when the (time dependent) outputs are averaged, (see Custom Output). The window-weight-function used is determined by the option WINDOW_FUNCTION

% ------------------ Coefficient-based Windowed Time Convergence Criteria -----------------------%
%
% Activate the windowed cauchy criterion
WINDOW_CAUCHY_CRIT = YES
%
% Specify convergence field(s)
CONV_WINDOW_FIELD= (TAVG_DRAG, TAVG_LIFT)
%
% Number of elements to apply the criteria
CONV_WINDOW_CAUCHY_ELEMS= 100
%
% Epsilon to control the series convergence
CONV_WINDOW_CAUCHY_EPS= 1E-3
%
% Number of iterations to wait after the iteration specified in  WINDOW_START_ITER.
CONV_WINDOW_STARTITER = 10
%
% Iteration to start the windowed time average
WINDOW_START_ITER = 500
%
% Window-function to weight the time average. Options (SQUARE, HANN, HANN_SQUARE, BUMP), SQUARE is default.
WINDOW_FUNCTION = HANN_SQUARE

Note: The options CONV_FIELD and CONV_WINDOW_FIELD also accept a list of fields, e.g. (DRAG, LIFT,...), to monitor. The solver will stop if all fields reach their respective stopping criterion (i.e. the minimum value for residuals or the cauchy series threshold for coefficients as mentioned above).