## Documentation Menu

## Input File ParametersRESTARTF
: Controls restart for flow field
RESTARTT : Controls restart for turbulence model. RNTCYC : Controls preconvergence of turbulence model. CURRENTLY DISABLED RESTART FILE : Name of restart file from which flow field and or turbulence MMESH : Number of meshes in mesh sequencing procedure. NTHREAD : Number of threads to be used in Open MP NCYC : Number of multigrid cycles NPRNT N MESH : Number of Mesh Levels in Multigrid Algorithm MESHLEVEL : Mesh level identifier. CFLMIN : Minimum (initial) CFL number. This value is ramped up over RAMPCYC cycles to its nominal value CFL or CFLC. RAMPCYC
: Number of cycles over which CFL is ramped (linearly) from CFLMIN to CFL or CFLC
TURBFREEZE : Enables freezing of turbulence model after TURBFREEZE cycles and continued convergence of flow equations for cases where overall convergence may be hampered by non-convergent turbulence model. CFL : CFL number (proportional to time step) for fine grid calculations. CFLV : No longer active. Leave at 1000. ITACC : Controls temporal accuracy for time dependent problems. INVBC : Controls treatment of wall velocities at slip (inviscid) boundaries. ITWALL : Controls wall temperature boundary condition (for Navier-Stokes flows). TWALL : Sets wall temperature for all insbc (Navier-Stokes ) wall boundaries when ITWALL = 1.0 VIS 1 : 1st order Artificial Dissipation Coefficient VIS 2 : 2nd order Artificial dissipation Coefficient. HFACTOR : Enthalpy damping coefficient. SMOOP : Implicit Residual Averaging Coefficient on Fine Grid. NCYCSM : Number of Cycles for Implicit Residual Averaging on Fine Grid. C1-C6 AND FIL1-FIL6 : Runge-Kutta or Hybrid Multi-Stage Scheme Coefficients. CFLC : CFL number for coarse grid levels. CFLVC : No longer functional. SMOOPC : Coarse level Implicit Residual Smoothing Parameter. NSMOOC : Number of Coarse level Implicit Residual Smoothing VIS0 : Coarse Mesh Level Artificial Dissipation Parameter. MGCYC : Multigrid Cycle Parameter. SMOOMG : Multigrid correction smoothing factor. NSMOOMG : Number of Multigrid correction smoothing cycles. ITURB : Parameter for selecting type of run and turbulence model. IWALLF : Wall treatment for turbulence models. WALLDIST : When using wall functions (IWALL=1) an estimated distance for the 1st point off the wall. CT1-CT6 : Iteration flags for turbulence model on FINE grid. CTC1-CTC6 : Iteration flags for turbulence model on COARSE grid. VIST0 : Coarse Level Dissipation Parameter for Turbulence Model. TSMOOMG : Smoothing parameter for turbulence model multigrid corrections. NTSMOOMG : Number of Multigrid correction smoothing cycles for turbulence model. MACH : Mach number for flow initialization and outer (far-field) boundary condition. Z-ANGLE : Angle of flow at outer boundary (in all cases) and for initialization of freestream (when no restart file is used: RESTARTF= 0.0) Y-ANGLE : Angle of flow at outer boundary (in all cases) and for initialization of freestream (when no restart file is used: RESTARTF= 0.0) RE : Reynolds number for the flow simulation. RE_LENGTH : Length scale (in grid dimensions) for Reynolds number specification. REF_AREA : Reference area (in grid dimensions) for force coefficient (CL, CD) definition and calculation. REF_LENGTH : Reference length (in grid dimensions) for moment coefficient (CM) definition and calculation. REF_MACH: XMOMENT : X location (in grid dimensions) for moment coefficient (CM) definition. YMOMENT : Y location (in grid dimensions) for moment coefficient (CM) definition ZMOMENT : Z location (in grid dimensions) for moment coefficient (CM) definition. ISPAN : Defines the coordinate system for force/moment calculation. MESH-DATA-FILE : Name of Partitioned Mesh File BCS FILE : The BCS file defines the boundary conditions for a particular run. TRANSITION-FILE : Transition may be specified using the optional transition file. RESTARTFRESTARTF = 0.0 : Initialize with freestream values (no restart for flow values) RESTARTF = 1.0 : Initialize flow field from restart file named under RESTART FILE (must be done on fine grid, which requires: MMESH=1, and MESHLEVEL=1.0) RESTARTF =-1.0: For time dependent problems, restart using 1st order time accuracy on first time step. For full second or higher order time accurate restarts, additional time levels are required in the restart file. If these are not available (because restart file was produced by steady-state run, or time dependent run at different time step size or using lower order time stepping scheme), a first order time accurate restart is required. This can be performed using RESTARTF=-1.0 If RESTARTF=1.0 is specified and the requisite time levels do not exist in the restart file, the restart will cause the code to stop execution. RESTARTTRESTARTT = 0.0 : Initialize turbulence model with freestream values (no restart for turbulence model) RESTARTT = 1.0 : Initialize turbulence model from restart file named under RESTART FILE (must be done on fine grid, which requires: MMESH=1, and MESHLEVEL=1.0) RNTCYCRun turbulence model RNTCYC cycles with frozen flow field prior to running combined flow field and turbulence model. Usual usage: Use RESTARTF=1.0 to read in a given flow field, and then preconverge turbulence model on this flow field. Can be used to study if turbulence model is cause of convergence difficulties. RESTART FILEModel fields are read in for initializing calculation. RESTART FILE is only active if RESTARTF=1.0 Otherwise, value is not read and may be left blank. MMESHNote this is NOT the same as multigrid procedure. Mesh sequencing is an outer loop which solves the flow on coarser grid levels and then interpolates this solution to a finer grid to be used as the initialization of the fine grid calculation. Note that there must be MMESH parameter lines under the heading line beginning with NCYC, NPRNT etc... Using grid sequencing (MMESH>1) provides more robust startup capablities for demanding cases by pre-converging the solution on coarser grids using a first-order discretization. NTHREADThis is only valid when running under OpenMP on shared memory architectures. Remember that most OpenMP implmentations require the setting of an environment variable (NCPUS, NCPU, OMP_NUM_THREADS, or OMP_NUMTHREADS) to achieve the requested level of parallelism. If the environment variable setting is smaller than the value of NTHREAD the solver will not execute. For pure MPI applications or single processor runs, set NTHREAD = 1.0 NPRNTResiduals are printed out to std out every cycle, but maximum residuals (and tubulence values) may also be output every NPRNT cycles. By doing this only every NPRNT cycles, the extra cost of seraching for the maximum residual values is minimized. Positive values of NPRNT print out maximum density residual and X-Y-Z location every NPRNT cycles. Negative values of NPRNT print out both density residuals/location and maximum eddy viscosity every abs(NPRNT) cycles. Note that there are MMESH lines under this heading. Each NPRNT entry corresponds to the number of cycles between max residual outputs on that grid level (out of MMESH grid levels) in the grid sequencing procedure. N MESHNote that there are MMESH lines under this heading. Each N MESH entry corresponds to the number of (multigrid) mesh levels on that grid level (out of MMESH grid levels) in the grid sequencing procedure. Typically, each extra line in the MMESH sequence will represent a finer grid, so the value of N MESH will be incremented by 1 going to each lower line (using all available grid levels on each MMESH) MESHLEVELNote that there are MMESH lines under this heading. Each MESHLEVEL entry defines the level of the finest mesh for this entry in the grid sequencing process. These levels are absolute, i.e. MESHLEVEL=1.0 always refers to the finest grid level (ie. the physical grid) in the grid file, while MESHLEVEL=2 refers to the next coarsest mesh (1st agglmoeration level) etc... While mesh sequencing is usually used to get a coarse grid solution as an initial guess for the fine grid problem, in principle, one can solve the flow on any grid level in any order. Each grid level starts with a flow field interpolated from the previous grid level. All grids except MESHLEVEL=1 are solved 1st order accurate (using coarse grid parameters such as CFLC, VIS0) since these are agglomerated levels. To run the finest level 1st order accurate, use MESHLEVEL= -1.0. This may also be helpful for smoothing out fine grid transient startup problems, although usually coarse grid solutions work well for this purpose. MESHLEVEL should not be confused with N MESH, which denotes the NUMBER of multigrid levels. Thus as MESHLEVEL decreases (goes to the fine grid) N MESH increases (we use more grid levels in the multigrid algorithm). CFLMIN: Note that there are MMESH lines under this heading. Each CFLMIN entry corresponds to the minimum CFL number for the problem on that grid level (out of MMESH grid levels) in the grid sequencing procedure. To avoid startup problems, small CFLMIN values on the first grids of the grid sequencing procedure are most useful. CFLMIN=0.01 or 0.1 work well, particularly for the first grid of the sequence. RAMPCYCNote that there are MMESH lines under this heading. Each RAMPCYC entry corresponds to the number of cycles used to ramp the CFL number on that grid level (out of MMESH grid levels) in the grid sequencing procedure. Ramping the CFL enhances robustness by avoiding startup problems. Typical values are some reasonable fraction of NCYC. TURBFREEZENote that there are MMESH lines under this heading. Each TURBFREEZE entry corresponds to the value used on that grid level (out of MMESH grid levels) in the grid sequencing procedure. TURBFREEZE = 0.0 omits any freezeing of the turbulence model. TURBFREEZE > NCYC also omits any freezing action. TURBFREEZE = -1.0 freezes turbulence model at initial values (no time stepping of turbulence model at all) Note only the value -1.0 produces total freeze, TURBFREEZE < -1.0 produces no freezing at all (as TURBFREEZE=0.0) A message is output at the cycle where the turbulence model becomes frozen. CFLDepends on scheme used (C1 C2 ... C6 coefficients). CFL = 1.0 for currently used 3 stage scheme in example above. CFL < 1.0 may be used for cases which diverge, but most often other strategies are more useful. CFLVNo longer active. Leave at 1000. ITACCITACC: Controls temporal accuracy for time dependent problems. ITACC = 0: used for steady-state simulations. ITACC = 1.0: Use BDF1 (1st order accurate backwards difference) time stepping scheme (low acuracy) ITACC = 2.0: Use BDF2 (2nd order accurate backwards difference) time stepping scheme (RECOMMENDED) ITACC = 3.0: Use BDF3 (3rd order accurate backwards difference) time stepping scheme (potentially unstable INVBCINVBC = 0.0 ---> Prescribe zero normal flux through slip wall boundary and perform no further treatment of wall velocties INVBC = 1.0 ---> Prescribe zero normal flux through slip wall boundary and set wall velocities tangential to wall boundary. For IBL cases, this is done ONLY at iblbc (IBL blowing) boundaries, NOT at regular slip boundaries where no blowing occurs. INVBC = 2.0 ----> Prescribe zero normal flux through slip wall boundary and set wall velocities tangential to wall boundary. For IBL cases, this is done BOTH at iblbc (IBL blowing) boundaries, AND at regular slip boundaries where no blowing occurs. ITWALLITWALL = 0.0 ---> Adiabatic wall ITWALL = 1.0 ---> Prescribed Temperature wall (at temp = TWALL) ITWALL = 2.0 ITWALL = 3.0 TWALLSets wall temperature for all insbc (Navier-Stokes ) wall boundaries when ITWALL = 1.0 VIS 1For subsonic and transonic flows, set VIS1 = 0.0 For flows with stronger shocks, values VIS1=1.0 up to 10.0 may help stability and supress oscillations near shock waves. However, non zero VIS1 values can reduce accuracy by increasing dissipation. Therefore, VIS1 = 0.0 is recommended except in the presence of strong shocks. VIS1 values are only active for IFLUX_TYPE=0 (matrix dissipation discretization), and only apply for fine grid of multigrid sequence. VIS1 values are ignored for all other discretizations. VIS 2The value of VIS2 depends on the particular discretization employed (i.e. IFLUX_TYPE parameter value). VIS2 values apply only to finest grid of the multigrid sequence. Matrix Artificial Dissipation: IFLUX_TYPE = 0.0 VIS2 = 20.0 is the standard value. Somewhat dissipative, but most robust and acceptable for most calculations. VIS2 = 10.0 can be used for more accurate (less dissipative) solutions when grid is of acceptable quality (thus avoiding robustness issues) Roe Upwind Scheme: IFLUX_TYPE = 1.0 VIS2 = 1.0 corresponds to the true Roe scheme. Values larger or smaller VIS2 values enhance or reduce (respectively) the dissipative part of the Roe scheme for added stability and reduced accuracy (or vice versa, respectively). Van-Leer Scheme: IFLUX_TYPE = 2.0 VIS2 values are ignored. HFACTORHFACTOR = 0.0 is the recommended value. Enthalpy damping is a technique which works only for Euler flows. In the current algorithm, the benefits are negligible, so enthalpy damping is not recommended. For inviscid flows, the value HFACTOR = 0.25 can be used to speed convergence, but gains are modest. SMOOPSMOOP = 0.0 is the recommended value: No residual averaging. (Residual Averaging has been superseeded by the point/line implicit algorithm) NCYCSMNCYCSM = 0.0 is the recommended value: No residual averaging. (Residual Averaging has been superseeded by the point/line implicit algorithm) C1-C6 AND FIL1-FIL6The combinations of these 12 coefficients determines the scheme used on each grid level for advancing the flow equations in (pseudo) time. C1-C6 are the traditional Runge-Kutta coefficients. FIL1-FIL6 are the coefficients for the dissipative terms. 3 stage and 5 stage schemes have both been used successfully. The 3 stage scheme coefficients are given as: C1 = 0.5321 C2 = 1.3711 C3 = 2.7744 FIL1 = 1.0 FIL2 = 1.0 FIL3 = 1.0 All other coefficients = 0.0 ( or simply not specified) and CFL = 1.0 Other schemes can be used, and these can be found in the literature. Note that the FIL1-6 values should be unity (1.0) for any corresponding non-zero value of the C1-6 coefficients. (Hybrid schemes where the dissipation terms are not evaluated at each stage are not implemented). CFLCThe coarse grid levels employ the same multi-stage time stepping scheme as the fine grid, and thus the CFL number should nominally be the same on coarse and fine levels. However, the option to use lower CFL numbers on the coarse levels is provided for cases where these levels are ill-conditioned. However, larger values of VIS0 generally work better for this task. CFLVCNo longer functional. SMOOPCRecommended value: SMOOPC = 0.0: No coarse level residual smoothing. NSMOOCCycles.Recommended value: NSMOOC = 0.0: No coarse level residual smoothing. VIS0The coarse (agglomerated) mesh levels employ a 1st order accurate dissipation formulation. A separate parameter is provided for specifying the level of dissipation on these coarse meshes. The value of VIS0 depends on the discretization (IFLUX_TYPE) used, and can be varied to influence robustness/speed of convergence. Matrix Artificial Dissipation (IFLUX_TYPE=0): VIS0 = 4.0 is the recommended value. Lower values (VIS0=2.0) speed convergence at the expense of robustness. Higher values (VIS0=6.0) improve robustness, particularly for ill-conditioned coarse levels, but slow convergence. Roe Upwind Scheme (IFLUX_TYPE = 1.0): VIS0 = 2.0 is the recommended value. The value VIS0 = 1.0 corresponds to the exact Roe scheme, and converges faster, but is less robust overall. Higher values can be used to improve robustness for ill-conditioned coarse grid levels, at the expense of speed of convergence. MGCYCMGCYC = 1 ---> Multigrid V-cycle MGCYC = 2 ---> Multigrid W-cycle (recommended SMOOMGWhen the coarse grid corrections are prolongated back to the fine grid in the multigrid algorithm, smoothing of the corrections is used to increase robustness. Recommended value: SMOOMG = 0.8. Higher values improve robustness but slow convergence. Lower values have the opposite effect. (Range of values : 0.2 - 1.2) NSMOOMGWhen the coarse grid corrections are prolongated back to the fine grid in the multigrid algorithm, smoothing of the corrections is used to increase robustness. Recommended value: NSMOOMG = 2.0 Higher values improve robustness but slow convergence. Lower values have the opposite effect. (Range of values : 1.0 to 4.0) ITURBITURB = 0 ---> Euler (inviscid flow) simulation ITURB = 1 ---> Laminar Navier Stokes (no turbulence model) ITURB = 2 ---> Interactive Boundary Layer simulation (IBL). Requires IBL module and compilation with IBL_ON ITURB = 4 ---> Spalart Allmaras Turbulence Model (recommended turbulence model) ITURB = 5 ---> K-Omega Turbulence model ITURB = 6 --->Menter SST Turblence model IWALLFIWALLF = 0 ---> Integrate to the wall. (Recommended setting) IWALLF = 1 ---> Use wall functions (no longer supported) WALLDIST(i.e. normal wall resolution) must be given in dimensions consistent with the grid units. Typical values for a grid normalized by the airfoil chord will be of the order of 1.e-04 for Reynolds numbers of several million in order to achieve Y+ values of ~100 at the wall. CT1-CT6dfThese coefficients should be either 1.0 or 0.0 CTn = 1.0 indicates the turbulence model is time-stepped (on the FINE grid) at the n-th stage of the time-stepping scheme used for the flow equations. CTn = 0.0 indicates the turbulence model is lagged (on the FINE grid) at the n-stage, ie. is not computed to save cpu time. Values other than 0.0 or 1.0 may cause instabilities. Values for n > number of stages in flow equations are ignored. CTC1-CTC6These coefficients should be either 1.0 or 0.0 CTCn = 1.0 indicates the turbulence model is time-stepped (on the COARSE grid) at the n-th stage of the time-stepping scheme used for the flow equations. CTCn = 0.0 indicates the turbulence model is lagged (on the COARSE grid) at the n-stage, ie. is not computed to save cpu time. Values other than 0.0 or 1.0 may cause instabilities. Values for n > number of stages in flow equations are ignored. Currently, k_Omega and SST models should be run with no coarse grid iterations (CTCn=0.0) Spalart Allmaras model can be used with or without coarse grid iterations. VIST0Artificial dissipation is added to the turbulence model on the coarse multigrid levels to enhance robustness.This has no effect on the final solution accuracy as it is only performed on the coarse levels and not the fine level. Recommended value : VIST0 = 2.0 Higher values tend to slow convergence. TSMOOMGWhen the coarse grid corrections are prolongated back to the fine grid in the multigrid algorithm, smoothing of the corrections is used to increase robustness. This is done for the turbulence model separately from the flow equations. Recommended value: TSMOOMG = 0.8 Higher values improve robustness but slow convergence. Lower values have the opposite effect. (Range of values : 0.2 - 1.2) NTSMOOMG.Smoothing of both flow equation and turbulence model corrections is done simultaneously. Thus, NTSMOOMG = NSMOOMG is REQUIRED. See NSMOOMG for details of parameter values. MACHFor freestream initialization (RESTARTF = 0.0) this Mach number is prescribed at the far-field boundary, and the entire flow field is initialized as a uniform flow with this Mach number. For a restart run (RESTARTF = 1.0) thisMach number prescribed at the far-field boundary, while the flow is initialized from the restart file. Z-ANGLEBecause of the various possiblities of defining the coordinate system, the terms incidence and yaw angles or not used. Rather, flow direction is specified based on the coordinate system. Z-ANGLE is the angle defined in the X-Y plane (the plane with normal vector in the Z axis). When Z is the spanwise direction (ISPAN=3), this corresponds to the incidence (angle of attack). When Y is the spanwise direction (ISPAN=2), this corresponds to the yaw angle. Y-ANGLEBecause of the various possiblities of defining the coordinate system, the terms incidence and yaw angles or not used. Rather, flow direction is specified based on the coordinate system. Y-ANGLE is the angle defined in the X-Z plane (the plane with normal vector in the Y axis). When Y is the spanwise direction (ISPAN=2), this corresponds to the incidence (angle of attack). When Z is the spanwise direction (ISPAN=3), this corresponds to the yaw angle. REThis Reynolds number is based on the length RE-LENGTH, which in turn is based on the grid dimensions. RE_LENGTHRE-LENGTH =1 .0 results in the value of RE being based on the grid dimension itself. REF_AREAReference area (in grid dimensions) for force coefficient (CL, CD) definition and calculation. REF_LENGTHReference length (in grid dimensions) for moment coefficient (CM) definition and calculation. REF_MACHXMOMENTX location (in grid dimensions) for moment coefficient (CM) definition YMOMENTY location (in grid dimensions) for moment coefficient (CM) definition ZMOMENTZ location (in grid dimensions) for moment coefficient (CM) definition. ISPANISPAN = 1: No woind axes definition. Forces are reported in X-Y-Z coordinate system only. ISPAN = 2: Y-coordinate direction is assumed to be in the spanwise direction. ISPAN = 3: Z-coordinate direction is assumed to be in the spanwise direction. The definitions of CL CD CM etc. depend on how the coordinate axes are defined. Definitions of incidence and yaw also depend on the coordinate axes. However, flow angles are specified directly in terms of the coordinate directions (Z-ANGLE, Y-ANGLE) so the user must be aware of which angle corresponds to incidence and yaw when setting these values. MESH-DATA-FILEThis is really a directory name, since partitioned files are stored in a directory with the name : mesh.partx, where x indicates the number of partitions in the directory. The directory files include: header.x, order.x, part.x and optionally ibl.x header.x are formatted readable files with grid size information. order.x are reordering files (integer) part.x files contain all grid information (ie. grid metrics etc) ibl.x files contain information for IBL runs. parta.x fles are also required for dynamic mesh cases. This requires preprocessing of mesh using pre_nsu3d (TYPE 2) for generating parta.x files. BCS-FILEThis file is optional and used only for boundary conditions with specifiable parameters, such as engine power boundary conditions where total pressure/temperature values may be specified. To avoid specifying the BCS file, remove the heading (OPTIONAL BCS FILE) and the line containing the file name. The boundary conditions are tagged to the grid in the pre_nsu3d phase. As such, the BCS file is not required since the boundary condition information is contained inside the MESH-DATA-FILE directory. However, the optional BCS file enables changing boundary condition types and parameters such as total pressure/temperature. Note that the boundary condition instances and their patch associations cannot be changed in the BCS file read in by the flow solver. This can only be done by going back through the pre_nsu3d pre-processing phase with a new BCS file. The BCS file read by the solver must therefore be compatible with the BCS file used in the pre_nsu3d phase and hence with the information inside the MESH-DATA-FILE directory. To avoid confusion, the patch associations in the bcs files read in by the solver at this stage are required to have "comment" characters: # preceeding the patch associations for the bc instances. A sample BCS file is provided inside each MESH-DATA-FILE directory called GRID.bcs. This file can either be used "in-situ" or copied to another location, and specified in the BCS FILE entry in the NSU3D input file. TRANSITION-FILEIf no file is specified, fully turbulent flow is assumed. To avoid specifying the Transition file, remove the heading (OPTIONAL TRANSITION FILE) and the line containing the file name. RESTARTF = 0.0 : Initialize with freestream values (no restart for flow values)
RESTARTF = 1.0 : Initialize flow field from restart file named under RESTART FILE (must be done on fine grid, which requires: MMESH=1, and MESHLEVEL=1.0) RESTARTF =-1.0: For time dependent problems, restart using 1st order time accuracy on first time step. For full second or higher order time accurate restarts, additional time levels are required in the restart file. If these are not available (because restart file was produced by steady-state run, or time dependent run at different time step size or using lower order time stepping scheme), a first order time accurate restart is required. This can be performed using RESTARTF=-1.0 If RESTARTF=1.0 is specified and the requisite time levels do not exist in the restart file, the restart will cause the code to stop execution. RESTARTT = 0.0 : Initialize turbulence model with freestream values (no restart for turbulence model)
RESTARTT = 1.0 : Initialize turbulence model from restart file named under RESTART FILE (must be done on fine grid, which requires: MMESH=1, and MESHLEVEL=1.0) |