Figure 1. Sample computational domain and grid
Chapter 2. INPUT DESCRIPTIONS: GENERAL CONTROL DATA
| TABLE OF CONTENTS | CLOSE MANUAL |
The VULCAN code input file provides many options for defining a computational domain, setting boundary conditions, initializing the flow, controlling the solution process, and selecting the information to be post-processed for plotting. Perhaps the best way to illustrate this is to start with an example of a simple geometry that illustrates many of VULCAN's capabilities and input flexibility. A three block grid is presented (see Chapter 11 for a discussion of domain decomposition terms) which provides a computational domain for solving the turbulent supersonic flow of hydrogen (H2 in block 2) and air (N2, O2 in block 1) over an infinitely thin splitter plate, and the resultant turbulent diffusion flame (block 3). In this example the domain is divided into 3 regions, where region 1 (containing block 1) is space marched, region 2 (containing block 2) is space marched and region 3 (containing block 3) is solved using the spatially elliptic solver in a time accurate manner.
Figure 1. Sample computational domain and grid
This sample input file is given with hyperlinks to relevant input description for navigational purposes within the input manual. It is not intended for actual use.
Table I. Sample input file
| $***************************************************************************$ $***************************************************************************$ $************** Test case for input gui that tries everything **************$ $***************************************************************************$ $***************************************************************************$ $******************* Beginning of general control data *********************$ $------------------- Parallel Processing Control data ----------------------$ PROCESSORS 1.0 (no. of processors to use if parallel processing) MESSAGE MODE 0.0 (message passing strategy: 0=standard, 1=buffered) $------------------- Geometric Model type ----------------------------------$ TWOD (twod, axisym, threed) $------------------- Grid File Data ----------------------------------------$ GRID FORMAT 3.0 (1=sb fmt, 2=sb unf, 3=mb fmt, 4=mb unf) GRID 0.0 (0=plot3d->3-D ; plot2d->2-D/axi, 1=plot3d->all) spltr_2d_cmb.grd GRID SCALING FACTOR 1.0 (mult. factor to convert grid units to meters) $------------------- Restart File Data -------------------------------------$ RESTART IN (input restart file name to follow) spltr_2d_cmb.rst RESTART OUT 50.0 (output restart file name to follow) spltr_2d_cmb.rst $------------------- Post-Processing Control -------------------------------$ PLOT ON 3.0 (1=sb fmt, 2=sb unf, 3=mb fmt, 4=mb unf) PLOT NODES (create PLOT3D files with data averaged to nodes) PLOT FUNCTION 7.0 (create PLOT3D function file with these variables) DENSITY VELOCITY PRESSURE TEMPERATURE MACH NO. EDDY VIS. RATIO MASS FRACTION 5 H2, H2O, N2, OH, O2 OUTPUT TIME HISTORY 10.0 (iteration interval between time history writes) spltr_2d_cmb.tim $------------------- Equation Set, Gas, and Reaction Model Control ---------$ GAS/THERMO MODEL 1.0 (0=calorically perfect, 1=thermally perfect) CHEMISTRY MODEL 1.0 (0=frozen, 1=finite rate, 2=n/a, 3=CARM, 4=ISAT) IMPLICIT CHEMISTRY 0.0 (0 or 1=analytical jacobian, 2=numerical jacobian) GLOBAL VISCOUS 0.0 (solve Navier-Stokes equation set) VISCOSITY MODEL 1.0 (n/a=power law, 1=Sutherlands law) CONDUCTIVITY MODEL 0.0 (0=Prandtl no., 1=Wassilej's law) UNIV. GAS CONST. 8314.34 NO. OF CHEMICAL SPECIES 7.0 ~your_login/Vulcan/Ver_6.1.0/Data_base/gas_mod.Lewis_1 N2 O OH O2 H H2 H2O 0.7686 0.0 0.0 0.2314 0.0 0.0 0.0 NO. OF CHEMICAL REACTIONS 7.0 ~your_login/Vulcan/Ver_6.1.0/Data_base/reac_mod.Larc_7x7 $------------------- Reference Condition Data ------------------------------$ ANGLE REF. FRAME 0.0 (0=alpha in xy plane, 1=alpha in xz plane) ALPHA 0.0 (angle of attack measured in degrees) NONDIM 1.0 (1=static conditions, 2=total conditions) MACH NO. 1.93e+00 STATIC TEMP. 1.00e+03 STATIC RHO 3.52e-01 LAM. PRANDTL NO. 0.72 LAM. SCHMIDT NO. 0.22 TURB. PRANDTL NO. 0.90 TURB. SCHMIDT NO. 0.90 $------------------- Turbulence Model Data ---------------------------------$ TURB. MODEL K-OMEGA TURB. INTENSITY 0.01 TURB. VISC. RATIO 0.10 BOUSSINESQ REY. STRESS 0.0 NO 2/3 RHOK IN REY. STRESS 0.0 $------------------- Runge-Kutta Scheme Control ----------------------------$ NSTAGE 3.0 (no. of Runge-Kutta stages) 0.3333333333333, 0.5, 1.0 RESMTYP 0.0 (res. smoothing: 0=none, 1=fix coef. 2=var coef.) $------------------- Boundary and Cut Control ------------------------------$ 0.0 BLOCKS 3.0 (no. of blocks) FLOWBCS 11.0 (no. of boundary conditions) CUTBCS 2.0 (no. of C(0) cut connectivity conditions) LAMINAR SUB-BLOCKS 2.0 (no. of laminar sub-blocks) IGNITION SUB-BLOCKS 1.0 (no. of ignition sub-blocks) TIME HISTORY I/O 1.0 (no. of time history sub-blocks) BLOCK CONFIG. 3.0 (no. of lines of block configuration input) BLK I-STRESS J-STRESS K-STRESS TURB REAC PLOT REGION 1 N T N Y N Y 1 2 N T N Y N Y 2 3 T T N Y Y Y 3 $**************************** Region 1 Control *****************************$ SOLVER ROE KAPPA LIMITER LIM-COEF. ENTROPY [U] ENTROPY [U+a] M/A 2 3 3 0 4 4 2.0 2.0 2.0 0.0 0.0 0.0 0.0 0.0 0.0 SM:START,STOP FMG:START,STOP VIGNERON LIMITER TURB-LIM SUB-STEP 1 64 1 5 0.95 1.0 1.0 N FMG-LVLS NITSCG1 NITSCG2 NITSFG 1ST-ORDER REL-RES ABS-RES 3 25 25 100 -2 -4.0 -5.0 MG-CYCLE COARSE GRIDS DQ-SMOOTH DQ-COEF. DAMP-MEAN DAMP-TURB V 2 0.1 0.25 1.0 0.5 TURB CONVECTION DT RATIO NON-EQUIL POINT-IMP COMP MODEL CG WALL BC 2ND 1.0 25.0 Y N STW SCHEME TIME STEP IT-STATS CFL-MIN ADP-CFL #CFL-VAL VISC-DT IMP-BC REG-REST DAF LOCAL 10 1.0 Y 3 Y N N 1 5 64 0.1 0.1 0.1 8.0 8.0 8.0 $**************************** Region 2 Control *****************************$ SOLVER LDFSS KAPPA LIMITER LIM-COEF. ENTROPY [U] ENTROPY [U+a] M/A 2 3 3 0 4 4 2.0 2.0 2.0 0.0 0.0 0.0 0.0 0.0 0.0 SM:START,STOP FMG:START,STOP VIGNERON LIMITER TURB-LIM SUB-STEP 1 64 1 5 0.95 1.0 1.0 M FMG-LVLS NITSCG1 NITSCG2 NITSFG 1ST-ORDER REL-RES ABS-RES 3 25 25 100 -2 -4.0 -5.0 MG-CYCLE COARSE GRIDS DQ-SMOOTH DQ-COEF. DAMP-MEAN DAMP-TURB V 2 0.1 0.25 1.0 0.5 TURB CONVECTION DT RATIO NON-EQUIL POINT-IMP COMP MODEL CG WALL BC 2ND 1.0 25.0 Y N STW SCHEME TIME STEP IT-STATS CFL-MIN ADP-CFL #CFL-VAL VISC-DT IMP-BC REG-REST DAF LOCAL 10 1.0 Y 3 Y N N 1 5 64 1 1 1 0.1 0.1 0.1 8.0 8.0 8.0 $**************************** Region 3 Control *****************************$ SOLVER HLLC KAPPA LIMITER LIM-COEF. ENTROPY [U] ENTROPY [U+a] E/A 3 3 3 2 2 2 2.0 2.0 2.0 0.0 0.0 0.0 0.0 0.0 0.0 FMG-LVLS NITSCG1 NITSCG2 NITSFG 1ST-ORDER REL-RES ABS-RES 3 25 25 200 -2 -4.0 -5.0 MG-CYCLE COARSE GRIDS DQ-SMOOTH DQ-COEF. DAMP-MEAN DAMP-TURB V 2 0.1 0.25 0.5 0.5 TURB CONVECTION DT RATIO NON-EQUIL POINT-IMP COMP MODEL CG WALL BC 2ND 1.0 25.0 Y Y STW SCHEME TIME STEP IT-STATS CFL-MIN ADP-CFL #CFL-VAL VISC-DT IMP-BC REG-REST DAF GLOBAL 10 0.5 Y 3 Y N N 1 50 500 0.5 2.5 5.0 !*********************** End of general control data ***********************! BC NAME BLK FACE PLACE DIR1 BEG END DIR2 BEG END IN-ORDER BC TYPE AIR-IN 1 I MIN J MIN MAX K MIN MAX 1 FIXED N2 O OH O2 H H2 H2O Rho U-Vel V-Vel W-Vel Pres T-int Mut/Mu 0.77 0.0 0.0 0.23 0.0 0.0 0.0 0.3516 1.2E3 0.0 0.0 -101325.0 0.01 1.0 OUTFLOW 1 I MAX J MIN MAX K MIN MAX 0 REGOUT2 BOTTOM 1 J MIN I MIN MAX K MIN MAX 0 EXTRAP WALL 1 J MAX I MIN MAX K MIN MAX 0 AWALLM H2-IN 2 I MIN J MIN MAX K MIN MAX 2 FIXED N2 O OH O2 H H2 H2O Rho U-Vel V-Vel W-Vel Temp T-int Mut/Mu 0.0 0.0 0.0 0.0 0.0 1.0 0.0 0.0246 3.8E3 0.0 0.0 1000.0 0.01 1.0 OUTFLOW 2 I MAX J MIN MAX K MIN MAX 0 REGOUT2 WALL 2 J MIN I MIN MAX K MIN MAX 0 AWALLM TOP 2 J MAX I MIN MAX K MIN MAX 0 EXTRAP PROFILE 3 I MAX J MIN MAX K MIN MAX 0 EXTRAP difflame.prof BOTTOM 3 J MIN I MIN MAX K MIN MAX 0 EXTRAP TOP 3 J MAX I MIN MAX K MIN MAX 0 EXTRAP CUT NAME BLK FACE PLACE DIR1 BEG END DIR2 BEG END IN-ORDER 1-3 1 I MAX J MIN MAX K MIN MAX 0 1-3 3 I MIN J MIN 65 K MIN MAX 3 2-3 1 I MAX J MIN MAX K MIN MAX 0 2-3 3 I MIN J 65 MAX K MIN MAX 4 LAM REG BLK DIR1 BEG END DIR2 BEG END DIR3 BEG END TRN-TYPE LE-BLK1 1 I MIN 15 J MIN MAX K MIN MAX LAMINAR LE-BLK2 2 I MIN 15 J MIN MAX K MIN MAX LAMINAR IGN REG BLK DIR1 BEG END DIR2 BEG END DIR3 BEG END T-IGNITE SPARK 3 I MIN 15 J 55 75 K MIN MAX 1800.0 TIM HIS BLK DIR1 BEG END DIR2 BEG END DIR3 BEG END TIMHIS 3 I MIN MAX J MIN MAX K MIN MAX |
GENERAL RULES:
1) Previous versions of VULCAN required that each line of the general input section of the input deck consist of a character string (enclosed by quotes), followed by a number. This number was required even when it had no meaning for the given input line. This restriction has now been removed to clarify the prescription of each input parameter. VULCAN now reads each line of the input deck as a pure character string, and parses the result to extract the required input information. This involves parsing out a keyword, or possibly a keyword followed by a number (at least two spaces must separate these items). In the following descriptions, the number (when applicable) is designated as REAL or INTEGER. An optional trailing descriptor is still allowed provided that it appears in the character string after all required information has been extracted.
Examples of valid input lines for specifying the number of processors:
'PROCESSORS' 2.0 (no. of processors to invoke) or
PROCESSORS 2.0 (no. of processors to invoke)
Examples of valid input lines for specifying the problem dimension:
'TWOD' 0.0 (twod, axisym, threed) or
TWOD (twod, axisym, threed)
2) Comment lines are designated by using $ as the first character of the character string. Note that a real number (or integer) is no longer required on comment lines. Any number of comment lines may be included.
Example:
'$------------------------ Geometric model type -------------------------$' 0.0 or
$------------------------ Geometric model type -------------------------$
3) The final line of the general input section is designated by a ! (this line must precede the boundary condition section of the input).
Example:
'!********************* End of general control data *********************!' 0.0 or
!********************* End of general control data *********************!
4) In the following input descriptions, an asterisk (*) indicates a default setting.
'PROCESSORS': REAL; The number of processors to be used in the simulation. It is permissible to have either fewer processors than blocks (more than one block on any given processor) or more processors than blocks in a given region (this might occur in multi-region simulations).
* 1.0
'MESSAGE MODE': REAL; Defines the message passing mode. A value of 0.0 will invoke the standard blocking MPI sends and receives. A value of 1.0 will invoke a buffered send with standard receive strategy. Typically, the standard mode will work best (fastest) for parallel_mpi (true MPI) installs, while the buffered mode tends to give better performance for non-proprietary MPI (e.g. MPICH) installs.
* 0.0
* 'THREED'; Solve the governing equations in 3-D Cartesian coordinates (X,Y,Z).
'AXISYM'; Solve the governing equations for axisymmetric flow without swirl (X,R).
'TWOD' ; Solve the governing equations in 2-D Cartesian coordinates (X,Y).
'GRID': REAL; Read and use a grid file which is named on the following line (full path may be included). The grid file may have one of two forms:
Table II. Input grid file PLOT2D/PLOT3D options
| GRID TYPE | : GEOMETRY TYPE INDICATOR AND FILE FORMAT/CONTENTS |
| 0.0=PLOT2D | : AXISYM or TWOD; arrays are in i,j form with x,y coordinates ONLY. |
| 1.0=PLOT3D | : THREED, AXISYM, or TWOD; arrays are in i,j,k form with x,y,z coordinates |
'GRID FORMAT': REAL; Format of the grid file to be read
1.0 = single block formatted PLOT3D style.
2.0 = single block unformatted PLOT3D style.
3.0 = multi-block formatted PLOT3D style.
* 4.0 = multi-block unformatted PLOT3D style.
'GRID SCALING FACTOR': REAL; Multiplication factor (greater than 0) for the grid coordinates to scale the grid to the desired units (for example, to convert a grid from inches to meters use 0.0254). The length scale definition used by UNIT REYNOLDS NO. must be consistent with GRID SCALING FACTOR (see "Reference Condition Data" below). When plot file is created ('PLOT ON' option in the "Output Control Data" section), the grid is output in the original unscaled units.
'C(0) TOLERANCE': REAL; Allowable block interface continuity tolerance (greater than 0) for grid interface connectivity checks performed by the solver. This option is only meant to be used in certain special scenarios, and as a result, it can not be accessed by the VULCAN G.U.I.
* 1.0e-04
'K-AXIS ORIENTATION': REAL; Used for 2-D and axisymmetric grids. Converts k-axis orientation for a left hand rule grid to k-axis orientation for a right hand rule grid. VULCAN assumes that the k direction is the same as the positive z direction. If the k direction is in the negative z direction, set 'K-AXIS ORIENTATION' to -1.0 to compensate. This option is only meant to be used in certain special scenarios, and as a result, it can not be accessed by the VULCAN G.U.I.
* 1.0 grid i, j, k coordinates follow right hand rule
-1.0 grid i, j, k coordinates follow left hand rule
'RESTART IN'; Restart file named on the following line (full path may be included). This file may or may not be read in depending on the Region settings (see REGION CONFIGURATION CONTROL).
'SERIAL INPUT RESTART FORMAT': Designates that the input restart file has the format of the serial code version (pre MPI and numbered by regions rather than blocks). If this option is specified then the output restart file MUST have a different name than the input restart file!
'RESTART ON GRID LEVEL': REAL; When restarting, restart calculation on grid level indicated. Grid levels are numbered in ascending order from coarsest to finest grid (e.g. if FMG-LVLS is 3, then 1.0=coarsest grid, 2.0=medium grid, 3.0=fine grid). The default is to restart on the grid level that the calculation was on when the restart file was written. This option is only meant to be used in certain special scenarios, and as a result, it can not be accessed by the VULCAN G.U.I.
'RE-INIT. BLOCKS': REAL; Re-initialize N blocks after reading the restart file. The actual block numbers to be re-initialized are specified on the following line as a comma separated integer list. This option is only meant to be used in certain special scenarios, and as a result, it can not be accessed by the VULCAN G.U.I.
'RE-INIT. BLOCKS' 3.0
3, 5, 7 (Blocks 3, 5, & 7 will be re-initialized after reading restart files)
'BLOCKS TO INIT. VEL. TO ZERO': REAL; Initialize the velocity to zero in N blocks. The actual block numbers to be re-initialized are specified on the following line as a comma separated integer list. This option is only meant to be used in certain special scenarios, and as a result, it can not be accessed by the VULCAN G.U.I.
'BLOCKS TO INIT. VEL. TO ZERO' 3.0
3, 5, 7 (Velocity will be initialized to zero in blocks 3, 5, & 7)
'INIT. BLENDING COEF.': REAL; Sets the percentage of the cells interior to a block that will be blended with the flow variables set by the boundary condition ghost cells as part of the flow initialization process. This blending is activated by specifying the B.C. NAME as BLEND (see Chapter 3 INPUT DESCRIPTION FOR BOUNDARY CONDITIONS for further details).
* 0.25 (Blends the B.C. 25 percent of the distance into a block., e.g. if BLEND were specified on a J min. boundary condition, and there were 100 cells in the J-direction in a block, the B.C. would be blended linearly with interior cells 1 through 25)
* 'VERBOSE OUTPUT'; Turn on detailed/verbose output state of the code as it runs.
'QUIET OUTPUT' ; Turn on limited/quiet output state of the code as it runs.
'WARNING MESSAGES': REAL; Controls the output of various warning messages
* 0.0 = all off
1.0 = wall function warning messages on.
2.0 = temperature warning messages on.
3.0 = update constraint violation warning messages on.
4.0 = all warning messages on.
'RESTART OUT': REAL; Write a restart file every N cycles to the file name (full path may be included) specified on the following line. If a non-positive value is specified, the restart file will we written when the simulation of each region has completed.
* 0.0 = only write a restart file after the simulation of each region has completed.
NOTE: The old 'RESTART OUT INTERVAL' keyword is still accepted for backwards compatability.
'PLOT ON': REAL; Turn on creation of PLOT3D style grid and flow solution files.
3.0 = multi-block formatted PLOT3D style.
4.0 = multi-block unformatted PLOT3D style.
* '32 BIT BINARY'; Output 32-bit (single precision) unformatted files.
'64 BIT BINARY'; Output 64-bit (double precision) unformatted files.
'PLOT NODES': Create plot files (with I-Blanking) with data averaged to the grid nodes.
'PLOT Q' Create plot files containing conserved variables. Filenames of files created are:
plot3d.g
plot3d.q
'PLOT FUNCTION': REAL; Create plot files containing N variables to be specified on the input lines immediately following. Filenames of files created are:
plot3d.g
Valid variable descriptor names are:
plot3d.f
VELOCITY: Cartesian velocity components
Example:
u,v for 2-D and axisymmetric flows
u,v,w for 3-D flows
GAMMA: Ratio of the specific heats
PRESSURE: Static pressure
GAUGE PRESSURE: Static pressure - reference pressure
TOTAL PRESS.: Total pressure
PITOT PRESS.: Pitot pressure
DENSITY: Static density
TOTAL DENS.: Total density
TEMPERATURE: Static temperature
TOTAL TEMP.: Total temperature
ENTHALPY: Static enthalpy
SENSIBLE ENTH.: Sensible static enthalpy
TOTAL ENTH.: Total enthalpy
ENTROPY: Mixture entropy
MACH NO.: Mach number
TURB. K.E.: Turbulent kinetic energy
TURB. DIS.: Turbulent (specific) dissipation rate
MENTER FUNCTION: Baseline blending function of Menter
DURBIN FUNCTION: Realizability constraint function of Durbin
CMUSTAR: Variable viscosity coefficient in the Gatski-Speziale ARS model
HYBRID FUNCTION: Hybrid RAS/LES blending function
TURB. TEMP. INTENSITY: rms temperature fluctuation divided by the temperature
TURB. COMP. INTENSITY: rms sum of the species mass fraction fluctuation
LAM. VIS.: Molecular viscosity
EDDY VIS. RATIO: Ratio of eddy viscosity to molecular viscosity
WALL DISTANCE: Distance to nearest wall
HEAT RELEASE: Heat release source term due to reaction
MASS FRACTION: Species mass fractions
two additional lines of information are required for this option:
1st line is an integer to specify the number of species to output
2nd line is a character string list that defines the species to output (at least 1 blank space should separate each species in the list)
(species names must match those in the CHEMICAL SPECIES INFORMATION section)
PRODUCTION RATE: Species production rates (mass-based)
two additional lines of information are required for this option:
1st line is an integer to specify the number of species to output
2nd line is a character string list that defines the species to output (at least 1 blank space should separate each species in the list)
(species names must match those in the CHEMICAL SPECIES INFORMATION section)
PLOT FUNCTION 4.0
TEMPERATURE
MACH NO.
EDDY VIS. RATIO
MASS FRACTION
2
H2O OH
'OUTPUT FLUXES'; Output inviscid flux data for each coordinate direction when post-processing. The flux data for each coordinate direction will reside in the sub-directory Flux_files.
'OUTPUT TIME AVERAGE': REAL; Form an ensemble-average of the data every N cycles as the code executes (only applicable when invoking a time-accurate integration strategy). The ensemble-averaged restart files are written out each time the standard restart files are written.
5.0 = form ensemble-averaged data every 5 cycles.
NOTE: The time-averaged data are written to restart files located in the sub-directory Time_files. The root name of these restart files is identical to the file name given after the 'RESTART OUT' line. If a full path is given for the restart file name, the path will be removed to force the time-averaged files to be placed in the Time_files directory).
NOTE: The post-processor will check for the existence of time-averaged data (located in the sub-directory Time_files) when the 'OUTPUT TIME AVERAGE' value is non-zero. If restart files are found in this directory for a given block number, then the data used for post-processing that block will be taken from the time-averaged restart file.
'OUTPUT H.O.T.': REAL; Add various higher-order ensemble-averaged terms to the ensemble-averaged restart file (only applicable when invoking a time-accurate integration strategy).
* 0.0 = skip output of higher order terms.
1.0 = output Reynolds stress and Reynolds scalar flux vectors.
2.0 = output scalar variances and covariances.
3.0 = output all 2nd order terms.
'OUTPUT TIME HISTORY': REAL; Write the time history file every N cycles as the code executes. Time history file named on the following line (full path may be included). Time histories are written over sub-domains defined in the TIME HISTORY I/O section.
10.0 = write time history every 10 cycles.
'F&M AVERAGING INTERVAL'; Average the force and moment history data over the most recent N cycles.
* 1.0 = do not average the force and moment histories.
'COMPUTE TOTAL PRESSURE LOSS'; Output total pressure loss information.
'COMPUTE COMBUSTION EFFICIENCY'; Output combustion efficiency based on the consumption of the least available reactant. If chemical reactions are not enabled, then this option outputs the mixing efficiency. At least 3 additional input lines (possibly as many as 5) must accompany this option:
'OXIDIZER SPECIES INDEX': REAL; Index of the species that contains the oxidizer.
The fuel & oxidizer indices are based on the species ordering in the CHEMICAL SPECIES INFORMATION section.
If this species is not a pure oxidizer (e.g. air), then the following input is also required:
'PURE OXIDIZER FRACTION': REAL; Fraction of the oxidizer species that is considered to be oxidizer.
* 1.0
'FUEL SPECIES INDEX': REAL; Index of the species that contains the fuel.
If this species is not a pure fuel, then the following input is also required:
'PURE FUEL FRACTION': REAL; Fraction of the fuel species that is considered to be fuel.
* 1.0
'STOICHIOMETRIC FUEL TO OXIDIZER MASS RATIO': REAL; Stoichiometric fuel to oxidizer ratio.
'COMPUTE FUEL PENETRATION HEIGHT'; Output fuel penetration height. The penetration height option must be used in conjunction with the 'COMPUTE COMBUSTION EFFICIENCY' option, and it currently is not available for reacting flows.
5) EQUATION SET AND SOLVER TYPE DATA
* 'GLOBAL VISCOUS': Solve the Navier-Stokes equations.
'GLOBAL EULER': Solve the Euler equations.
'MARCHING VISCOUS': Solve the parabolic Navier-Stokes equations.
'MARCHING EULER': Solve the parabolic Euler equations.
'LINEAR SOLVER CONVERGENCE CRITERIA': REAL; Specifies the convergence criteria for the linearization error of the variable update for the ILU scheme.
*-1.0 = stop the linear equation solves once the error norm has been reduced by 1 order of magnitude
'REPORT LINEAR SOLVER HISTORY'; Outputs the convergence history for the linearization error of the variable update of the ILU scheme.
'DISS. RED. FAC.': REAL; Scalar reduction factor for the numerical dissipation matrix of the ROE scheme. Valid values range from -1.0 to +1.0 (negative values activate the shock sensor).
* 1.0
'DYN. DISS. FAC.': REAL; Relaxation parameter controlling the shock sensor when the dissipation reduction factor is invoked. Valid values range from 0.0 to 1.0.
* 0.01
'PERIODIC BODY FORCE': REAL; Applies a body force to the streamwise momentum equation and the energy equation to model fully-developed flow with periodic boundary conditions (useful in LES or hybrid RAS/LES applications). The streamwise direction is indicated by the value associated with this keyword:
1.0 = denotes X as the streamwise direction
2.0 = denotes Y as the streamwise direction
3.0 = denotes Z as the streamwise direction
This option is limited in that it can only be used when there is one block per processor. Due to the limited scope of this option, it can not be accessed by the VULCAN G.U.I.
6) ANGLE OF ATTACK INFORMATION
'ANGLE REF. FRAME': REAL; Reference frame for angle of attack and yaw.
* 0.0 = xy plane and xz plane (typical of internal flows)
1.0 = xz plane and xy plane (typical of external flows)
'ALPHA': REAL; Valid range 0.0 <= ALPHA(degrees) <= 180.0. If the angle reference frame indicator is:
* 0.0 = ALPHA is measured in the xy plane, counter clockwise relative to the negative x axis
1.0 = ALPHA is measured in the xz plane, counter clockwise relative to the negative x axis
'BETA': REAL; Valid range 0.0 <= BETA(degrees) <= 180.0.If the angle reference frame indicator is:
* 0.0 = BETA is measured in the xz plane, counter clockwise relative to the negative x axis
1.0 = BETA is measured in the xy plane, counter clockwise relative to the negative x axis
Figure 2. Angle of attack reference frames.
'DIRECTION COSINE METHOD'; Reference velocity components computed based on the specification of direction cosines (in lieu of specifying angle of attack and angle of yaw), followed by the direction cosines for each coordinate direction;
'DIR_COS(U)': direction cosine for the x-velocity component.
'DIR_COS(V)': direction cosine for the y-velocity component.
'DIR_COS(W)': direction cosine for the z-velocity component.
'MOMENT REF. X': REAL; Reference X coordinate for moment calculations.
* 0.0
'MOMENT REF. Y': REAL; Reference Y coordinate for moment calculations.
* 0.0
'MOMENT REF. Z': REAL; Reference Z coordinate for moment calculations.
* 0.0
'INTEGRATION REF. LENGTH': REAL; A reference length (meters) used by the post-processor to convert integrated forces and moments to force and moment coefficients.
'INTEGRATION REF. AREA': REAL; A reference area (m^2) used by the post-processor to convert integrated forces and moments to force and moment coefficients.
'INTEGRATION X SCALE FACTOR': REAL; Scaling factor used to scale the x-coordinates for the integrated force and moment data.
* 1.0
'INTEGRATION Y SCALE FACTOR': REAL; Scaling factor used to scale the y-coordinates for the integrated force and moment data.
* 1.0
'INTEGRATION Z SCALE FACTOR': REAL; Scaling factor used to scale the z-coordinates for the integrated force and moment data.
* 1.0
'INTEGRATION REF. PRESSURE': REAL; A reference pressure (Pascals) used by the post-processor during the integration of the boundaries for the pressure and momentum integrals. The pressure that is integrated will be Pstatic - P_int_ref.
*'INCLUDE SLIP WALLS'; Consider all slip surfaces in the surface force and moment integrations.
'EXCLUDE SLIP WALLS'; Omit all slip surfaces in the surface force and moment integrations.
'GAS/THERMO MODEL': REAL; Type of gas and thermodynamics model to be used
* 0.0 = Calorically perfect gas (constant gamma).
1.0 = Mixture of thermally perfect gases.
'UNIV. GAS CONST.': Universal gas constant in MKS units [(kg-m^2/sec^2)/(kmol-K)].
* 8314.34
'MIN. STATIC TEMP.': Minimum allowable static temperataure (in Kelvin).
* 10.0
'MAX. STATIC TEMP.': Maximum allowable static temperataure (in Kelvin).
* 1500.0 (calorically perfect flows) or
the maximum temperature allowed by the thermodynamic property curve fits (thermally perfect flows)
CHEMISTRY MODEL: REAL; Type of chemical kinetics model to be used.
* 0.0 = frozen (no reaction).
1.0 = finite rate.
2.0 = n/a.
3.0 = Computer Automated Reduced Mechanism (CARM).
4.0 = CARM with In-Situ Automated Tabulation (ISAT).
'IMPLICIT CHEMISTRY': REAL; Use point implicit treatment of source term in species transport equations.
1.0 = use analytical Jacobian (0.0 also employs the analytical Jacobian).
* 2.0 = use numerical Jacobian.
'VISCOSITY MODEL': REAL; Type of model to be used to compute molecular viscosity.
* 1.0 = Sutherlands law (if multicomponent gas, Wilke's law is used).
'CONDUCTIVITY MODEL': REAL; Type of model used to compute molecular conductivity.
* 0.0 = Prandtl number
1.0 = Wassiljewa's law (for multicomponent gas only).
'SPEC. DIFF. MODEL': REAL; Type of diffusion model used for molecular viscous transport of species.
* 0.0 = Fickian diffusion model.
10) CHEMICAL SPECIES INFORMATION
VULCAN allows for an arbitrary mixture of thermally perfect gases.
The number of chemical species must be specified. The thermodynamic and transport properties of the gas species are modeled using curve fits, which have coefficients that are read from chemical species database files supplied with the code (see Chapter 10 CHEMICAL SPECIES THERMODYNAMIC AND TRANSPORT MODEL INPUT).
'NO. OF CHEMICAL SPECIES': REAL; Number of chemical species requiring transport equations.
The next line consists of the file name (full path may be included) of the database file to be used.
The species names are given on the next line (with at least 1 blank space separating each species).
The names must match the abbreviations used in the database that was chosen.
The mass fractions that are used to form the reference gas mixture of each species are given on the next line (real numbers).
Example:
NO. OF CHEMICAL SPECIES 7.0
~your_path_here/gas_mod.Lewis_2
N2 O OH O2 H H2 H2O
0.7686 0.0 0.0 0.2314 0.0 0.0 0.0
Three database files are provided such that:
1) gas_mod.Lewis_1: Uses 1-interval 7-coefficient curve fits created by B. McBride from NASA Lewis, for temperatures between 300 and 5,000 K.
2) gas_mod.Lewis_2: Uses 2-interval 7-coefficient curve fits created by B. McBride from NASA Lewis, for temperatures between 200 and 6,000 K.
3) gas_mod.Lewis_3: Uses 3-interval 9-coefficient curve fits created by B. McBride from NASA Lewis, for temperatures between 200 and 20,000 K.
11) CHEMICAL REACTION INFORMATION
VULCAN allows for an arbitrary chemical kinetic mechanism.
The number of chemical reactions and the kinetic model data must be specified along with the number of chemical species as described in the preceding section.
If finite rate chemistry is chosen (see CHEMISTRY MODEL), then the kinetic model data is specified through a kinetic model database file. Several models are provided with the code. If the supplied files do not cover the desired kinetic model, the user may construct a new file using the description in Chapter 9 CHEMICAL REACTION MODEL INPUT.
'NO. OF CHEMICAL REACTIONS': REAL; Number of chemical reactions to be modeled.
The next line consists of the file name (full path may be included) of a kinetic model database file that is consistent with the species specified in the NO. OF CHEMICAL SPECIES input line.
NO. OF CHEMICAL REACTIONS 7.0
~your_path_here/reac_mod.Larc_7x7
If the Computer Automated Reduction Mechanism (with or without ISAT) is chosen (see CHEMISTRY MODEL), then the kinetic model data is specified through a user-supplied file (CARM.F). Only species that are tracked by the reduced model (i.e. species solved by transport equations) need to be specifed in the NO. OF CHEMICAL SPECIES input line.
If the Computer Automated Reduction Mechanism with In-Situ Automated Tabulation is chosen (see CHEMISTRY MODEL), then the following parameters that control the processing of the ISAT can be specified:
'ISAT PARAMETERS': REAL; The number of ISAT parameters to be specified on the following lines:
'MAX. TREE NODES': REAL; The maximum number of nodes in the ISAT tree structure (default value is 50000).
'ERROR TOLERANCE': REAL; The error tolerance used by ISAT (default value is 0.05). Recommended values are 0.01 < REAL < 0.05.
'CHEMICAL TIME SCALE': REAL; An estimate of the chemical time scale used by ISAT to define reference values (default value is 1.0e-05).
'F0(SPECIES)': REAL; Reference mass fraction value for species SPECIES (default value is 0.01). SPECIES must be a species specified in the NO. OF CHEMICAL SPECIES input line, and the value specified should roughly correspond to the maximum value expected in the computational domain.
'F0(TEMPERATURE)': REAL; Reference temperature (default value is 1000 K). The value specified should be some representative temperature in the reaction zone.
'F0(PRESSURE)': REAL; Reference pressure (default value is 100000 Pa). The value specified should be some representative pressure in the reaction zone.
12) REFERENCE CONDITION DATA
Options are for A) calorically perfect gas, B) mixture of thermally perfect gases.
A) Reference conditions for calorically perfect gas
'NONDIM': REAL; The type of data (static or total) given to define the reference conditions.
* 1.0 = static conditions used for reference condition determination and boundary conditions, followed by:
'GAMMA': REAL; Ratio of specific heats.
'MACH NO.': REAL; Mach number.
and any 3 of the following variables:
'STATIC RHO': REAL; Static density in kg/m^3.
'GAS CONSTANT': REAL; Gas constant for perfect gas law in m^2/(sec^2-K).
'STATIC TEMP.': REAL; Static temperature in Kelvin.
'STATIC PRESS.': REAL; Static pressure in Pascals.
2.0 = total conditions used for reference condition determination and boundary conditions, followed by:
'GAMMA': REAL; Ratio of specific heats.
'MACH NO.': REAL; Mach number.
and any 3 of the following variables:
'TOTAL RHO': REAL; Total density in kg/m^3.
'GAS CONSTANT': REAL; Gas constant for perfect gas law in m^2/(sec^2-K).
'TOTAL TEMP.': REAL; Total temperature in Kelvin.
'TOTAL PRESS.': REAL; Total pressure in Pascals.
For both static conditions and total conditions (1.0 and 2.0), the following lines are also required if viscous flows are considered:
'UNIT REYNOLDS NO.': REAL; Unit Reynolds number (consistent with GRID SCALING FACTOR).
'SUTHERLANDS LAW S0': REAL; Constant S in Sutherlands law (units of Kelvin).
'LAM. PRANDTL NO.': REAL; Laminar Prandtl number.
'TURB. PRANDTL NO.': REAL; Turbulent Prandtl number.
If UNIT REYNOLDS NO. <= 0.0, then the value entered for the Reynolds number is ignored and the following 2 lines are required:
'SUTHERLANDS LAW MU0': REAL; Constant mu0 in Sutherlands law (units of kg/(m-sec)).
'SUTHERLANDS LAW T0': REAL; Constant T0 in Sutherlands law (units of Kelvin).
B) Reference conditions for a mixture of thermally perfect gases
'NONDIM': REAL; The type of data (static or total) given to define the reference conditions.
* 1.0 = static conditions used for reference condition determination and boundary conditions, followed by:
'MACH NO.': REAL; Mach number.
and any 2 of the following variables:
'STATIC RHO': REAL; Static density in kg/m^3.
'STATIC TEMP.': REAL; Static temperature in Kelvin.
'STATIC PRESS.': REAL; Static pressure in Pascals.
2.0 = total conditions used for reference condition determination and boundary conditions, followed by:
'MACH NO.': REAL; Mach number.
and any 2 of the following variables:
'TOTAL RHO': REAL; Total density in kg/m^3.
'TOTAL TEMP.': REAL; Total temperature in Kelvin.
'TOTAL PRESS.': REAL; Total pressure in Pascals.
For both static condition and total condition specifications, the following lines are also required if viscous flows are considered:
'LAM. PRANDTL NO.': REAL; Laminar Prandtl number.
'LAM. SCHMIDT NO.': REAL; Laminar Schmidt number.
'TURB. PRANDTL NO.': REAL; Turbulent Prandtl number.
'TURB. SCHMIDT NO.': REAL; Turbulent Schmidt number.
'TURB. MODEL': Defines the beginning of turbulence model definition section. The turbulence model to be used is specified on the next input line. No number is required on the model specification line.
* 'LAMINAR': Laminar flow (no turbulence model selected).
'SPALART': One-equation model of Spalart et al.
'K-EPSILON': Low Reynolds number k-epsilon model of Abid and Speziale.
'K-OMEGA': Wilcox k-omega model (1998 version) without the Pope correction term.
'K-OMEGA_POPE': Wilcox k-omega model (1998 version) with the Pope correction term.
'LOW RE K-OMEGA': Low Reynolds number Wilcox k-omega model (1998 version) without the Pope correction term.
'MENTER': Blended (Wilcox 1988 k-omega / Jones Launder k-epsilon) two-equation model of Menter.
'MENTER-SST': Shear stress transport model variant of the Menter two-equation model.
'SMAGORINSKY': Constant coefficient Smagorinsky sub-grid scale model with van Driest wall damping.
NOTE: The y+ value required by the van Dries wall damping term [1.0 - exp(-y+/26)] is evaluated at each grid cell as the minimum value relative to any wall attached to the grid lines that define the given cell. No search is performed outside of the block that owns the grid cell.
Example:
TURB. MODEL
MENTER
*'BOUSSINESQ REY. STRESS'; Reynolds stresses modeled using Boussinesq model.
'G.S. ALG. REY. STRESS'; Explicit algebraic Reynolds stress model of Gatski and Speziale. Available only with K-OMEGA and K-EPSILON models.
'THIN LAYER SOURCE TERMS'; This option allows the thin layer specification in the BLOCK CONFIG. section to be applied to the turbulent source terms.
'DURBIN REALIZABILITY': REAL; This option forces the turbulent time scale to be realizable based on Durbin's model. Available with all two-equation models. Valid values for the realizability scaling factor are 0.50 <= REAL <= 1.0.
* Default behaviour is that the model is turned off.
'NO 2/3 RHOK IN REY. STRESS'; This option neglects the 2/3*rho*k terms that appear in the normal Reynolds stresses. Use this option only with the BOUSSINESQ REY. STRESS model.
* Default behavior includes the 2/3*rho*k in the normal Reynolds stresses
*'SMAGORINSKY CONSTANT': REAL; Constant used for the SGS viscosity when the Smagorinsky model (SMAGORINSKY) is invoked.
* 0.012
'TURB. INTENSITY': REAL; Intensity of reference turbulent velocity fluctuations relative to the mean reference velocity field.
* 0.01
'TURB. VISC. RATIO': REAL; Ratio of reference turbulent viscosity to the reference molecular viscosity.
* 0.10
'DISABLE WALL MATCHING SUB-LAYER'; Disables the near wall blending of the wall function boundary condition with the integrate to the wall expressions. This has alleviated high frequency residual error oscillations for some flows. This option is only meant to be enabled in certain special scenarios, and as a result, it can not be accessed by the VULCAN G.U.I.
'INIT. MIN. DIST.'; Compute the distance to the nearest wall. Can be used to force the code to recompute the distribution when restarting. You might want to do this if you adapted the grid and were going to restart from the "old" solution. This option is only meant to be enabled in certain special scenarios, and as a result, it can not be accessed by the VULCAN G.U.I.
'INITIAL BOUNDARY LAYER THICHNESS': REAL; This option allows for the specification of an initial boundary layer thickness (in meters) for no-slip surfaces.
* 0.0
'MAX. ALLOWABLE MUT/MU': REAL; This option allows the eddy viscosity to molecular viscosity ratio to be clipped at some maximum value (on the order of 10,000 or greater). This option is only meant to limit the eddy viscosity during rapid flow transients, and as a result, it can not be accessed by the VULCAN G.U.I.
'HYBRID-LES': REAL; Defines the desired hybridization strategy for blending the RAS and LES equation sets.
* 0.0 = No hybrid model (pure RAS turbulence model selected).
1.0 = Detached Eddy Simulation (2-equation variant) model of Strelets.
2.0 = Variant of the Limited Numerical Scales (LNS) model of Batten et al.
3.0 = Hybrid model based on the formulation of Baurle and Edwards.
Note that the HYBRID-LES model 2.0 differs from the LNS model of Batten et al. in that the SGS viscosity is based on the SGS TKE rather than the value obtained from a Smagorinsky closure.
'HYBRID-LES CVIS': REAL; Defines the SGS viscosity constant for the hybrid RAS/LES model. Used with HYBRID-LES models 2.0 and 3.0. Also used to specify the SGS viscosity constant for the Smagorinsky model if the LES-SMAG option is chosen.
'HYBRID-LES CDIS': REAL; Defines the SGS TKE dissipation constant for the hybrid RAS/LES model. Used with HYBRID-LES models 1.0 and 3.0. This coefficient is the inverse of the standard DES constant when model 1.0 is invoked.
'HYBRID-LES CDIF': REAL; Defines the SGS TKE diffusion constant for the hybrid RAS/LES model. Used with HYBRID-LES model 3.0.
'HYBRID-LES ALPHA': REAL; Defines the coefficient (α) that controls the y+ value where the RAS/LES blending function switches from RAS to LES. Used with HYBRID-LES model 3.0.
'HOMOGENEOUS-I'; Assumes homogeneous turbulence in the i-coordinate direction. This disables consideration of the i-direction arc length component when defining the sub-grid length scale.
'HOMOGENEOUS-J'; Assumes homogeneous turbulence in the j-coordinate direction. This disables consideration of the J-direction arc length component when defining the sub-grid length scale.
'HOMOGENEOUS-K'; Assumes homogeneous turbulence in the k-coordinate direction. This disables consideration of the K-direction arc length component when defining the sub-grid length scale.
NOTE: An isotropic definition for the sub-grid length scale is enabled by specifying all coordinate directions as homogeneous.
'TIME SCALE SGS'; Uses the product of the time step and the maximum of the mean velocity magnitude or rms velocity fluctuation as a limiting factor when determining the SGS length scale.
15) TURBULENCE-CHEMISTRY MODEL DATA
'TURB. CHEM. MODEL': Defines the beginning of turbulence chemistry model definition section. The turbulence chemistry interaction model to be used is specified on the next input line. No number is required on the model specification line.
'TEMPERATURE PDF': Enables a presumed PDF for temperature fluctuations.
'COMPOSITION PDF': Enables the multi-variate presumed PDF of Girimaji for composition fluctuations.
'TEMP./COMP. PDF': Enables a presumed PDF for temperature and a presumed PDF for composition fluctuations.
'EDDY DISSIPATION': Enables the eddy dissipation concept (EDC) of Magnussen and Hjertager.
'EDDY DISSIPATION WITH FINITE RATE': Enforces the minimum reaction rate given by the eddy dissipation model and any supplied finite rate data (see Chapter 9 CHEMICAL REACTION MODEL INPUT).
NOTE: The EDC models apply only to one-way (forward only) reactions.
Example:
TURB. CHEM. MODEL 0.0
EDDY DISSIPATION
'GAUSSIAN FUNCTION'; The presumed PDF of temperature is a Gaussian function.
'BETA FUNCTION'; The presumed PDF of temperature is a Beta function.
'TURB. TEMP. INTENSITY': REAL; The reference turbulence intensity based on temperature fluctuations.
* 0.01
'TURB. COMP. INTENSITY': REAL; The reference turbulence intensity based on mass fraction fluctuations.
* 0.01
'ENERGY VARIANCE CONSTANT': REAL; The constant for the destruction term of the energy variance equation solved when temperature fluctuations are accounted for with a presumed PDF.
* 2.0
'SPECIES VARIANCE CONSTANT': REAL; The constant for the destruction term of the species variance sum equation solved when composition fluctuations are accounted for with a presumed PDF.
* 2.0
'DISABLE SPECIES VARIANCE CHEMICAL SOURCE'; Disables the chemical source term that appears in the equation for the species mass fraction variance sum.
'1ST EDC CONSTANT': REAL; The constant "A" for the EDC model. A zero value implies no reaction, and very large values imply chemical equilibrium.
* 4.0
16) RUNGE-KUTTA SCHEME DEFINITION
These options provide for control of the Runge-Kutta scheme if R-K is chosen as the time integration method for any region. Runge Kutta is not recommended for use with space marching.
'CFLSTAR': REAL; Maximum stable CFL of explicit scheme on fine grids.
* 2.5
'NSTAGE': REAL; Number of Runge-Kutta stages to be used in scheme, to be followed by the coefficients.
* 5.0 with the following coefficients:
0.2742, 0.2067, 0.5020, 0.5142, 1.0
Example:
NSTAGE 3.0
0.3333333333, 0.5, 1.0
'RESMTYP': REAL; Type of implicit residual smoothing to be used.
0.0 = None.
1.0 = Constant coefficient.
* 2.0 = Variable coefficient.
NOTE: Residual smoothing will be disabled if a time-accurate integration strategy is invoked.
'RESMPHI': REAL; Coefficient for constant coefficient residual smoothing:
0.50 < RESMPHI < 0.75
* 0.50
or minimum coefficient for variable coefficient smoothing.
0.01 < RESMPHI < 0.10
* 0.01
'RESMPSI': REAL; Constant for variable coefficient residual smoothing.
0.125 < RESMPHI < 0.25
* 0.25
The grid is divided into blocks, which may be grouped as regions. A region consists of a group of complete (not partial) blocks.
'FLOWBCS': REAL; The number of boundary conditions (see Chapter 3 INPUT DESCRIPTION FOR BOUNDARY CONDITIONS for a description of the boundary condition inputs).
* 0.0
'CUTBCS': REAL; The number of C(0) or grid point continuous block-to-block interface conditions (see Chapter 4 INPUT DESCRIPTION FOR C(0) BLOCK INTERFACE (CUT) CONDITIONS for a description of the C(0) block interface condition inputs).
* 0.0
'PATCHBCS': REAL; The number of non-C(0) or grid point discontinuous block-to-block interface conditions (see Chapter 5 INPUT DESCRIPTION FOR NON-C(0) BLOCK INTERFACE (PATCH) CONDITIONS for a description of the non-C(0) block interface condition inputs).
* 0.0
'PATCH FILE': The path and/or name of the file (on the following line) that is to be created to contain the patch interpolation coefficients computed by the patch pre-processor.
NOTE: This line only needs to exist when PATCHBCS > 0.0.
'BCGROUPS': REAL; The number of boundary condition groupings (see Chapter 3 INPUT DESCRIPTION FOR BOUNDARY CONDITIONS for a description of the boundary condition grouping inputs).
* 0.0
'BCOBJECTS': REAL; The number of boundary condition objects (i.e. groups of boundary condition groupings). Further details on the specification of boundary condition objects is given in Chapter 3 INPUT DESCRIPTION FOR BOUNDARY CONDITIONS.
* 0.0
'BLOCKS': REAL; The number of blocks in the input grid.
* 1.0
'LAMINAR SUB-BLOCKS': REAL; The number of regions where turbulence is suppressed in the domain. If this number is greater than 0, further input must follow the General Control Data section of the input file (see Chapter 6 INPUT DESCRIPTION FOR LAMINAR SUB-BLOCKS for a description of the laminar sub-block inputs).
* 0.0
'IGNITION SUB-BLOCKS': REAL; The number of regions where the static temperature (or energy source) is set to a prescribed value in the domain. If this number is greater than 0, further input must follow the General Control Data section of the input file (see Chapter 7 INPUT DESCRIPTION FOR IGNITION SUB-BLOCKS for a description of the ignition sub-block inputs).
* 0.0
'TIME HISTORY I/O': REAL; The number of regions where time histories are desired. If this number is greater than 0, further input must follow the General Control Data section of the input file (see Chapter 8 INPUT DESCRIPTION FOR TIME HISTORY SUB-BLOCKS for a description of the time history sub-block inputs).
* 0.0
18) BLOCK CONFIGURATION CONTROL
'BLOCK CONFIG.': REAL; The number of input lines (see below) describing the configuration or state of the viscous terms, turbulence model, and chemical kinetic model for each block of the input grid. There is no default, and there must be at least one of these lines, as described below.
The first line is a user defined comment line. The following lines (the number of lines being equal to the BLOCK CONFIG. number) are configuration lines. Each line must contain the following items, in this order:
BLK I-STRESS J-STRESS K-STRESS TURB REAC PLOT REGION
where:
BLK = Block indicator:
0 = All blocks will be set to this configuration as an initialization.
>0 = Only this block number will be set.
I-STRESS J-STRESS K-STRESS; Three character strings that indicate the method used to compute the derivatives used in the viscous flux terms. The I, J, and K-directions each use one of the following
N = No derivatives are evaluated.
T = Face derivatives are evaluated using a simplified stencil.
F = Face derivatives are evaluated using a full stencil.
NOTE 1: If the flow is 2-D or axisymmetric, the code will (re)set the K-direction viscous flag to N. If I, J, and K directions are all N the Euler equations will be solved in the block.
NOTE 2: If the space marching scheme is being used, the code will (re)set the streamwise viscous flag to N.
TURB; If a turbulence model is being used, this is used to turn the turbulence model on or off in the block:
N = No - turbulence model is off
Y = Yes - turbulence model is on
REAC; If a chemical kinetics model is being used, this is used to turn the kinetics model on or off in the block:
N = No - chemical kinetics model is off
Y = Yes - chemical kinetics model is on
PLOT; The PLOT3D files for this block are to be merged into the aggregate PLOT3D files:
N = No - do not merge the files for this block into the aggregate PLOT3D files
Y = Yes - merge the files for this block into the aggregate PLOT3D files
REGION; Region number that the block belongs to.
NOTE 3 Older versions of VULCAN required the specification of the SOLVER type in the block configuration section just prior to the specification of the REGION number. VULCAN will accept this older format for backward compatability, but the solver type (which is region specific rather than block specific) should now be specified in the REGION CONFIGURATION CONTROL section (see SOLVER) of the input deck.
Example 1) Two blocks in a single region with laminar, non-reacting flow.
BLOCKS 2.0
BLOCK CONFIG. 2.0
BLK I-STRESS J-STRESS K-STRESS TURB REAC PLOT REGION
0 N T T Y 1
Example 2) Two blocks, each in a separate region, with turbulent, non-reacting flow.
BLOCKS 2.0
BLOCK CONFIG. 2.0
BLK I-STRESS J-STRESS K-STRESS TURB REAC PLOT REGION
1 T T T Y Y 1
2 T T T Y Y 2
Example 3) Two blocks with laminar, reacting flow. Block 1 has the I-direction viscous terms deactivated.
BLOCKS 2.0
BLOCK CONFIG. 2.0
BLK I-STRESS J-STRESS K-STRESS TURB REAC PLOT REGION
1 N T T Y Y 1
2 T T T Y Y 2
Example 4) Six blocks with turbulent, reacting flow. Blocks 2, 5 & 6 in Region 2 are solved with a full viscous stencil with turbulence and reactions activated, blocks 1, 3, and 4 are in Region 1 and solved using a reduced viscous stencil. Note that the first line, with BLK set to 0, initializes all blocks to the setting in this line. The blocks to be configured differently are specified separately.
BLOCKS 6.0
BLOCK CONFIG. 4.0
BLK I-STRESS J-STRESS K-STRESS TURB REAC PLOT REGION
0 F F F Y Y Y 2
1 N N N N N Y 1
3 T T N Y Y Y 1
4 T T N Y Y Y 1
19) REGION CONFIGURATION CONTROL
For each group of blocks (or region) there must be a group of input lines.
Each group must begin with a user comment line designating the region:
Example:
$******************** REGION 1 solved space marching ********************$
The following input lines (1-8) each consist of a comment line followed by a line (or lines) consisting of the values for the appropriate parameters.
Line 1: Defines the solver type, convective flux scheme, and convective flux parameters for the I, J, and K directions (in I,J,K order).
Line 2: Space marching instructions for the marching (I) direction. I-direction values in line 1 above (other than KAPPA) are ignored. (This line should only be present in regions solved using the space marching scheme)Example 1: Active parabolic region using the Roe upwind scheme:
SOLVER ROE KAPPA LIMITER LIM-COEF. ENTROPY [U] ENTROPY [U+a]
M/A 2 3 3 0 4 4 2.0 2.0 2.0 0.0 0.0 0.0 0.0 0.0 0.0Example 2: Inactive elliptic region using the Edwards low dissipation flux split scheme:
SOLVER LDFSS KAPPA LIMITER LIM-COEF. ENTROPY [U] ENTROPY [U+a]
E/I 3 3 3 4 4 4 2.0 2.0 2.0 0.0 0.0 0.0 0.0 0.0 0.0Example 3: Active elliptic region using the Edwards preconditioned flux split scheme
SOLVER PRECOND KAPPA LIMITER LIM-COEF. ENTROPY [U] ENTROPY [U+a]
E/A 3 3 3 4 4 4 2.0 2.0 2.0 0.5 0.0 0.0 0.0 0.0 0.0The specification of the solver (SOLVER) used for the region consists of two parts separated by a slash (/). The 1st part designates the solver type, and the 2nd part designates whether the region is active or inactive:
M = parabolic (space-marching in the I-direction)
E = elliptic
and
I = inactive
A = activeValid inviscid flux constructions are as follows:
ROE : Upwind scheme using the Roe approximate Riemann solver.
VANLEER : vanLeer flux vector split scheme.
LDFSS : Edwards Low dissipation flux split scheme.
HLLC : Toro Low dissipation flux split scheme.
PRECOND : Edwards low Mach no. preconditioned flux split scheme.
NO : No inviscid flux evaluation (useful for point chemical kinetics).Valid MUSCL interpolation coefficient (KAPPA) schemes are as follows:
1 = First order scheme
2 = Second order fully upwind scheme
3 = Second order kappa = 1/3 scheme
4 = Second order Fromme schemeIf using the space marching algorithm, any KAPPA value other than 1 in the I-direction gives 2nd order fully upwind space marching.
Valid flux limiter (LIMITER) options are as follows:
0 = None
1 = Minmod (TVD)
2 = vanLeer (TVD)
3 = vanAlbada
4 = Smooth limiter (only for use with KAPPA = 3.0 or 4.0)
5 = Koren
6 = Minmod (ENO)
7 = vanLeer (ENO)NOTE: The ENO limiters (5 & 6) do not telescope across cut boundaries due to the added stencil length required by these limiters.
Valid limiter coefficient (LIM-COEF.) values (required for the smooth limiters only) are:
1.0e-3 < LIM-COEF. < 1.0e+8 (larger values reduce the level of flux limiting relative to smaller values).Valid convective eigenvalue entropy fix (ENTROPY [U]) values are flux scheme specific.
If the ROE scheme is chosen, the input values given for this section are used to alleviate shock/grid alignment (carbuncle) problems. For this scenario, valid values are:
-0.5 <= ENTROPY [U] < 0.0: Constant coefficient limiting.
0.0 < ENTROPY [U] <= 1.0: Adaptive coefficient limiting based on pressure gradients. (Recommended method)
If the LDFSS scheme is chosen, the input values given for this section are used to control a blend of the low dissipation flux split scheme with the vanLeer method. Any value > 0.0 enables the blend in the specified coordinate direction.
If the PRECOND scheme is chosen, the input values given for this section are used to limit the minimum velocity for the low-velocity preconditioning scheme:
0.0 < ENTROPY [U] <= 1.0 : Constant coefficient minimum velocity limiter.
-1.0 <= ENTROPY [U] < 0.0 : Darmofal's variable coefficient minimum velocity limiter.
NOTE: This quantity is a global (i.e. used for all coordinate directions) parameter for the PRECOND scheme, so only the first value (I-direction) is required.Valid acoustic eigenvalue entropy fix (ENTROPY [U+a]) values used to alleviate the expansion shock problem (for use with the ROE scheme only) are:
-0.5 <= ENTROPY [U+a] < 0.0: Fixed coefficient scheme.
0.0 < ENTROPY [U+a] <= 1.0: Adaptive coefficient scheme. (Recommended method)
Line 3: Grid sequencing and iteration control data.Example: SM:START,STOP FMG:START,STOP VIGNERON LIMITER TURB-LIM SUB-STEP
1 64 1 5 0.95 1.0 1.0 MSTART,STOP: INTEGER; Designates the I index range (cells) to consider. If STOP is greater than the number of marching direction grid cells, the code will reset STOP to the maximum number of marching direction grid cells.
FMG:START,STOP: INTEGER; Controls the range of I-planes to perform coarse-to-fine sequencing. If STOP is greater than the number of marching direction grid cells, the code will reset STOP to the maximum number of marching direction grid cells.
VIGNERON: REAL; Safety factor for the streamwise parabolic operator.
0.9 < VIGNERON < 0.99MEAN-LIM: REAL; Controls space marching streamwise limiting of the mean flow equations. Smaller values imply more limiting.
0.5 < MEAN-LIM < ∞ (1.0 is the recommended value)TURB-LIM: REAL; Controls space marching streamwise limiting of the turbulence equations. Smaller values imply more limiting.
0.5 < TURB-LIM < ∞ (1.0 is the recommended value)SUB-STEP: CHARACTER STRING; Controls space marching sub-stepping. VULCAN can either space march using the input grid, such that 30 I grid planes will result in 29 space marching steps or it can linearly subdivide the input grid cells according to a sub-step schedule specified in the CFL section of the input giving more resolution in the space marching direction.
Valid Options are:
N = None, requires no further input.
M = Manual, requires a sub-step table in the time marching section (see Time stepping scheme control data).
Example: FMG-LVLS NITSCG1 NITSCG2 NITSFG 1ST-ORDER REL-RES ABS-RESLine 4: Multi-grid control data.
3 25 25 100 -2 -4.0 -6.0 FMG-LVLS: INTEGER; The number of grid levels to be used in coarse to fine sequencing of the solver.
1 <= FMG-LVLS <= 5NITSCG#: INTEGER; The number of iterations to be run on each grid level repeated FMG-LVLS minus 1 times. In ascending order where the first is on the coarsest grid and the last on the finest grid.
NITSFG: INTEGER; The number of iterations to be run on the finest grid level.
1ST-ORDER: INTEGER; Sets the point, designated either by iteration number or by coarse grid level, at which to change from a first order scheme to a higher order scheme. Negative values designate grid levels, positive values designate iteration numbers.
Example: If there are 3 grid levels (fine grid [level 0], medium grid [level 1] and coarse grid [level 2]), then
0 switches from 1st order to higher order when solving on the coarse grid [coarse grid level 2]. -1
switches from 1st order to higher order when solving on the medium grid [coarse grid level 1].
-2
switches from 1st order to higher order when solving on the finest grid [coarse grid level 0].
REL-RES,ABS-RES: REAL; Residual error norm criteria for halting execution on the current plane (space marching) or the entire region (elliptic).
REL-RES = Orders of magnitude reduction of the residual relative to the maximum residual (-4.0 sets a convergence criteria of 4 orders of magnitude reduction of the L2 norm of the residual relative to the max. L2 norm of the residual).
ABS-RES = Orders of magnitude of the absolute residual (-6.0 sets a convergence critera when the Log(base10) of the L2 norm of the absolute residual is less than or equal to -6.0).
Example: MG-CYCLE COARSE GRIDS DQ-SMOOTH DQ-COEF. DAMP-MEAN DAMP-TURBLine 5: Turbulence model control data.
V 2 0.1 0.25 1.0 0.5MG-CYCLE: CHARACTER STRING;
I = Use coarse to fine sequencing with no multi-grid
V = V cycle multi-grid algorithm
W = W cycle multi-grid algorithmCOARSE GRIDS: INTEGER; The number of coarse grids to be used in the multi-grid process. The value entered here is also used to determine the storage required for the coarse grid levels, and as a result, should always be no smaller than FMG-LVLS minus 1.
0 <= COARSE GRIDS <= FMG-LVLS minus 1DQ-SMOOTH: REAL; Coefficient used for implicit smoothing of coarse grid corrections.
0.10 < DQ-SMOOTH < 0.30DQ-CORR.: REAL; Used in two ways:
1) Maximum allowable coarse grid correction (for multi-grid) as a percentage of the current value of the conserved variable.
2) Maximum allowable conserved variable update as a percentage of the current value of the conserved variable. A positive value constrains the magnitude of the update by [ABS(DQ-CORR) * (current value of Q)] only when the update violates a realizability constraint. A negative value constrains the magnitude of the update by [ABS(DQ-CORR) * (current value of Q)] at all times.
0.25 < ABS(DQ-CORR) < 0.75DAMP-MEAN: REAL; Minimum allowable coefficient for damping the multi-grid forcing function for the mean flow equations.
0.1 < DAMP-MEAN < 1.0DAMP-TURB: REAL; Minimum allowable coefficient for damping the multi-grid forcing function for the turbulence model equations.
0.1 < DAMP-TURB < 0.5
Line 6: Time stepping scheme control data.Example: TURB CONVECTION DT RATIO NON-EQUIL POINT-IMP COMP MODEL CG WALL BC
2ND 1.0 25.0 Y N WMFTURB CONVECTION: CHARACTER STRING; Spatial order of accuracy used to treat convective terms of the turbulence equations.
1ST = 1st order
2ND = 2nd orderDT-RATIO: REAL; Ratio of turbulence time-step to mean flow time-step.
0.1 < DT RATIO <= 1.0NON-EQUIL: REAL; Maximum allowable degree of non-equilibrium behavior in the turbulence. Only active for 2-equation models.
10.0 < NON-EQUIL < ∞POINT-IMP: CHARACTER STRING; Turbulence source term point implicit treatment.
Y = Turbulence source term point implicit treatment on.
N = Turbulence source term point implicit treatment off.COMP-MODEL: CHARACTER STRING; Compressibility correction model for the 2-equation models.
Y = Compressibility correction model on.
N = Compressibility correction model off.CG WALL BC: CHARACTER STRING; Coarse-grid wall turbulence boundary conditions.
WMF = Wall matching function.
STW = Solve to the wall.
Example 1: For an elliptic region.
SCHEME TIME STEP IT-STATS CFL-MIN ADP-CFL #CFL-VAL VISC-DT IMP-BC REG-REST
DAF LOCAL 10 1.0 Y 3 Y N Y
1 100 1000 <- Absolute iteration no.
1.0 6.0 6.0 <- CFL no.Example 2: For a space marching region with manual sub-stepping.
SCHEME TIME STEP IT-STATS CFL-MIN ADP-CFL #CFL-VAL VISC-DT IMP-BC REG-REST
DAF LOCAL 10 1.0 Y 3 Y N Y
1 5 100 <- Space marching plane no.
1 2 2 <- Number of sub-steps per input grid cell
1.0 6.0 6.0 <- Initial CFL no. on the plane
3.0 6.0 6.0 <- Final CFL no. on the planeExample 3: For an elliptic region using a time accurate Runge-Kutta scheme.
SCHEME TIME STEP IT-STATS CFL-MIN ADP-CFL #CFL-VAL VISC-DT IMP-BC REG-REST
R-K DELTAT 10 1.0 Y 3 Y N Y
1 100 1000 <- Absolute time step no.
5.0e-7 1.0e-6 2.0e-6 <- time step size (seconds)Example 4: For an elliptic region using the ILU scheme.
SCHEME TIME STEP IT-STATS CFL-MIN ADP-CFL #CFL-VAL VISC-DT IMP-BC REG-REST
ILU LOCAL 10 1.0 Y 3 Y N Y
SWEEP-DIR JAC_UPDATE START NUM-SLVS RELAX
0 0 0 2 0.95
1 100 1000 <- Absolute iteration no.
1.0 1.0e6 1.0e6 <- CFL no.
Example 5: For an elliptic region using a time accurate DAF (CFL based) dual-time stepping scheme.
SCHEME TIME STEP IT-STATS CFL-MIN ADP-CFL #CFL-VAL VISC-DT IMP-BC REG-REST
DAF SUBIT1 10 1.0 Y 3 Y N Y
1 5 10 <- Absolute iteration no.
1.0 100.0 100.0 <- Sub-iteration CFL no.
TIME STEP SUB-ITS RES-RED TIME-ORDER C-N RELAX
5.0e-7 5 -3.0 2ND 0.50Example 6: For an elliptic region using a time accurate DAF (Pseudo-time step) dual-time stepping scheme.
SCHEME TIME STEP IT-STATS CFL-MIN ADP-CFL #CFL-VAL VISC-DT IMP-BC REG-REST
DAF SUBIT2 50 1.0 N 3 Y N Y
1 5 10 <- Absolute iteration no.
1.0 10.0 10.0 <- Sub-iteration CFL no.
TIME STEP SUB-ITS RES-RED TIME-ORDER C-N RELAX
5.0e-7 5 -3.0 2ND 0.50Example 7: For an elliptic region using a time accurate ILU (CFL based) dual-time stepping scheme.
SCHEME TIME STEP IT-STATS CFL-MIN ADP-CFL #CFL-VAL VISC-DT IMP-BC REG-REST
ILU SUBIT1 10 1.0 Y 3 Y N Y
SWEEP-DIR JAC_UPDATE START NUM-SLVS RELAX
0 0 0 2 0.95
1 100 1000 <- Absolute iteration no.
1.0 1.0e6 1.0e6 <- Sub-iteration CFL no.
TIME STEP SUB-ITS RES-RED TIME-ORDER C-N RELAX
5.0e-7 5 -3.0 2ND 0.50SCHEME: CHARACTER STRING; Temporal advancement scheme to be used.
DAF = Diagonalized Approximate Factorization.
ILU = Incomplete LU. Relaxation and Jacobian update controls must be specified in the ILU relaxation and Jacobian update control section.
R-K = Runge-Kutta. Stage coefficients and residual smoothing options must be specified in the RUNGE-KUTTA SCHEME DEFINITION section.
NOTE: The Runge-Kutta scheme is not recommended for steady-state simulations.TIME STEP: CHARACTER STRING; Type of method used to obtain the time step.
LOCAL = Local time step scheme.
GLOBAL = Global time step scheme.
DELTAT = Specified time step scheme.
SUBIT1 = Dual-time stepping scheme with CFL values used for the sub-iterations.
SUBIT2 = Dual-time stepping scheme with time-step scaling factors used for the sub-iterations.
NOTE: Dual-time stepping options are only compatible with the DAF and ILU schemes, and require additional control data (see Dual-time stepping scheme and sub-iteration control data).IT-STATS: INTEGER; Iteration/time step interval at which the statistics about solver performance are written as part of the output file.
10 = Iteration statistics written every 10 iterations.CFL-MIN: REAL; CFL number used as lower limit when ADP-CFL is activated. When running difficult cases, set this value to a small number (on the order of 0.1).
ADP-CFL: CHARACTER STRING; Turns on a normalized pressure gradient-based time stepping scheme which decreases the CFL number near large pressure gradients.
N = Scheme off.
Y = Scheme on (highly recommended).#CFL-VAL: INTEGER; Number of iteration and CFL number table entries.
A schedule of iteration vs. CFL (or delta time) values is required on the next two lines when the region is elliptic. A third and possibly fourth line will be present for space marching regions.
The first line is a list of numbers (INTEGER) corresponding to either:
a) Iteration or cycle number when the region is solved elliptically
b) Plane number when the region is solved space marching
The second line (USED ONLY WHEN SPACE MARCHING AND WHEN SUB-STEP IS SET TO M) is a list of numbers (INTEGERS) corresponding to the number of sub-steps to take relative to the plane number specified in the line above it.
The third line is a list of numbers (REAL) corresponding to either:
a) Current CFL numbers (ELLIPTIC REGIONS) with LOCAL or GLOBAL time stepping.
b) Current time step increment (seconds) (ELLIPTIC REGIONS) with DELTAT time stepping.
c) Initial CFL numbers on the current plane (SPACE MARCHING REGIONS).
d) Current CFL number of the sub-iteration (ELLIPTIC REGIONS) using the DAF or ILU scheme in conjunction with SUBIT1 dual-time stepping.
e) Current time-step scaling factor of the sub-iteration (ELLIPTIC REGIONS) using the DAF or ILU scheme in conjunction with SUBIT2 dual-time stepping.
The fourth line (USED ONLY WHEN SPACE MARCHING) is a list of numbers (REAL) corresponding to the final CFL numbers on the current plane.The code linearly interpolates between values set by this input to determine a CFL number (or time-step) at each cycle/iteration.
VISC-DT: CHARACTER STRING; Consider the viscous eigenvalues when computing the time step
Y = Use viscous eigenvalues.
N = Do not use viscous eigenvaluesIMP-BC: CHARACTER STRING; Use implicit boundary conditions (available only for the ILU scheme).
Y = Use implicit boundary conditions.
N = Do not use implicit boundary conditions.REG-REST: CHARACTER STRING; Read the restart file for this region.
Y = Read restart file for this region.
N = Do not read restart file for this region.
Line 7: ILU relaxation and Jacobian update control. (Use only for regions solved using the ILU scheme)
Example: SWEEP-DIR JAC_UPDATE START NUM-SLVS RELAX
0 0 0 2 0.95SWEEP-DIR: INTEGER; Relaxation sweep direction.
0 = Sweep direction of each grid block is aligned with the direction of the smallest spectral radius.
1 = Sweep direction is I.
2 = Sweep direction is J.
3 = Sweep direction is K.
-# = Full 3-D ILU scheme.JAC-UPDATE: INTEGER; Controls how often the Jacobians are updated. This parameter improves the efficiency of the ILU scheme by reducing the overhead associated with evaluating the Jacobians.
0 = Default algorithm that updates the Jacobian less frequently as the solution converges.
<0 = Aggressive algorithm that updates the Jacobian less frequently as the solution converges.
>0 = Jacobian updated at user specified iteration intervals.START: INTEGER; Iteration number to start utilizing the update Jacobian schedule. The Jacobian is updated at every iteration cycle prior to this point (this input is ignored if one of the automated algorithms is selected for JAC-UPDATE).
NUM-SLVS: INTEGER; Number of linear algebra solves using the planar ILU method. This parameter reduces the factorization error associated with multi-dimensions and "broken" implicit operators resulting from block-to-block interfaces. (Recommended value is 5).
NOTE: The convergence history of the linearization error can be monitored via the keyword REPORT LINEAR SOLVER HISTORY.
NOTE: The convergence criteria of the linearization error is specified via the keyword 'LINEAR SOLVER CONVERGENCE CRITERIA'.RELAX: REAL; Relaxation coefficient to enhance robustness.
0.50 <= RELAX <= 0.95
Line 8: Dual-time stepping scheme and sub-iteration control data. (Use only for elliptic regions solved using the DAF or ILU scheme with dual-time stepping)
Example: TIME STEP SUB-ITS RES-RED TIME-ORDER C-N RELAX
5.0e-7 5 -3.0 2ND 0.50TIME STEP: REAL; Physical time step in seconds.
SUB-ITS: INTEGER; Maximum number of sub-iterations to be performed.
SUB-ITS >= 5RES-RED.: REAL; Orders of magnitude to reduce the residual error during the sub-iteration process relative to the initial value.
-2.0 <= RES-RED <= -6.0TIME-ORDER: CHARACTER STRING; Method used to form the temporal differencing term.
1ST: First order backward difference (1st order time accuracy).
2ND: Second order backward difference (2nd order time accuracy).
C-N: Crank-Nickolson scheme (2nd order time accuracy).C-N RELAX: REAL; Relaxation coefficient for the Crank-Nickolson scheme.
0.25 <= C-N RELAX <= 0.50
At this point, a line designating the end of the General Control Data section is required. See "General Rules" at the beginning of this chapter.
Example:
!************************* End of general control data *************************!
| TABLE OF CONTENTS | CLOSE MANUAL |