Problem data refers to all the information required for performing the analysis and it does not concern any particular Tdyn module. Problem data also differs from the previous definitions of conditions and materials properties, which are assigned to different entities. Some examples of general problem data are the type of solution algorithm used by the solver, the value of the time step, convergence conditions and so on.
Tdyn Problem and Solver Data window can be started from Data > Problem Data .
This group of data refers to the selection of problems to be solved with Tdyn.
Solve Fluid : Select this option if you are going to solve any fluid problem. If this option is not selected, any defined fluid domain will be ignored in the solution of the problem.
Solve Fluid Flow : Select this option if you are going to solve fluid flow (RANSE) problem. This option will only be available in RANSOL module
Solve Temperature : Select this option to solve a heat transfer problem in a fluid. If this option is not selected, the temperature problem in fluid domains will be ignored in the solution process. This option will only be available in HEATRANS module
Solve Species Concentration : Select this option to solve a species advection problem in fluid. If this option is not selected, the species advection problem in fluid domains will be ignored in the solution. This option will only be available in ADVECT module.
Solve Phi Problems : Select this option to solve any user defined PDE (phi variables) problem in fluid. If this option is not selected, the user defined PDEs problem in fluid domains will be ignored in the solution. This option will only be available in URSOLVER module.
Solve Odd LevelSet : Select this option to solve free surface problems in fluid based on ODD level set. This option will only be available in ODDLS module.
Solve Mesh Deformation : Select this option to apply mesh deformation algorithms and apply Arbitrary Lagrangean Eulerian (ALE) solvers in fluid. This option will only be available in ALEMESH module.
Solve Transpiration : Select this option to solve a transpiration free surface problem in fluid. If this option is not selected, the transpiration free surface problem in fluid domains will be ignored in the solution. This option is only available in NAVAL module of Tdyn 3D.
Solve Solid : Select this option if you are going to solve any solid problem. If this option is not selected, any defined solid domain will be ignored in the solution of the problem.
Solve Solid Flow : Select this option if you are going to solve fluid flow problem in a solid (flow in porous media). This option will only be available in RANSOL module
Solve Temperature : Select this option to solve a heat transfer problem in a solid. If this option is not selected, the temperature problem in solid domains will be ignored in the solution process. This option will only be available in HEATRANS module
Solve Species Concentration : Select this option to solve a species advection problem in solid. If this option is not selected, the species advection problem in solid domains will be ignored in the solution. This option will only be available in ADVECT module.
Solve Phi Problems : Select this option to solve any user defined PDE (phi variables) problem in solid. If this option is not selected, the user defined PDEs problem in solid domains will be ignored in the solution. This option will only be available in URSOLVER module.
Solve Mesh Deformation : Select this option to apply mesh deformation algorithms and apply Arbitrary Lagrangean Eulerian (ALE) solvers in fluid. This option will only be available in ALEMESH module.
Solve Structural Problem : Select this option to solve structural problem in solids. This option will only be available in RAMSOLID module.
Number of Steps : Number of steps of the simulation. Total physical time to be simulated will be Number of Steps x Time increment . Recommended value to achieve steady state is:
Number of Steps ≥ 1000·dt·V/LD
where dt is the time increment and V, LD the characteristic velocity and length.
Time Increment : Time step of the simulation. Total physical time to be simulated will be Number of Steps x . The recommended value is:
dt = C·LD /V
where dt is the time increment, V, LD the characteristic velocity and length and 0.1 < C < 0.01.
For transient solutions a value of dt calculated as 1/10 to 1/100 of the period or characteristic time of the problem is usually more appropriate.
Time increment may also be defined by a global function (see Function Syntax section for further information). Units of the time step of the simulation are given in the menu next to this field.
Max Iterations : Maximum number of iterations of the non-linear algorithm for solution of the problem. Recommended values come from 3 to 10, depending on the value of the convergence norms (see Modules Data section).
Remarks:
In some cases the algorithm may not converge in the initial time-steps, due to the start up process, resulting in the appearing of a warning message More than...number...iterations may be necessary . If only the steady state is of interest, this message may be simply ignored, otherwise Max Iterations value should be increased.
Initial Steps : During first Initial Steps some controls are carried out in the algorithm in order to stabilise the problem during the start up process. It is strongly recommended to define Initial Steps about 10% of the Number of Steps in problems with free surface transpiration.
Start Up Control : if activated, during first Initial Steps the start up process is smoothed. This can be done by creating a adequate acceleration in the flow (Speed ), by smoothly increasing the time increment (Time ) or Both .
Restart : if On , the restart file is used to define the initial data. The Restart file taken will be ‘ProblemName.flavia.rst’. This file is automatically written by Tdyn with the rest of the results.
Output Step : Each Output Step time steps the results will be written to disk.
Remarks:
This value will control the size of the results file.
Output Start : The results will be written each Output Step time steps after Output Start steps.
Remarks:
This value will control the size of the results file.
Results File : Type of the results file (Binary, Ascii or EnsightGold). Binary type should be selected in order to minimise the size of the results file.
Initial Data : Mark to write in the results file some general data of the initial operations.
Velocity : Mark to write velocity field in the results file.
Velocity Stress Tensor : Mark to write velocity stress tensor field in the results file.
Pressure : Mark to write pressure field in the results file.
Pressure Gradient : Mark to write pressure field in the results file.
Total Pressure : Mark to write total pressure field in the results file (including hydrostatic component).
Density : Mark to write fluid density field in the results file.
Viscosity : Mark to write viscosity field in the results file.
Wall Law Traction : Mark to write wall stress given by the Law of the Wall (if exits) in the results file.
Tau Parameter : Mark to write tau parameter (local Courant number) field in the results file.
Eddy Viscosity : Mark to write eddy viscosity field in the results file.
Eddy Kinetic Energy : Mark to write eddy kinetic energy field in the results file.
Epsilon : Mark to write epsilon (turbulence variable) field in the results file.
Omega : Mark to write omega (turbulence variable) field in the results file.
K Tau : Mark to write kτ variable (of K_KT turbulence model) field in the results file.
Real Velocity : Mark to write real velocity on bodies.
Temperature : Mark to write temperature field in the results file.
Temperature Gradient : Mark to write temperature gradient field in the results file.
Heat Flux : Mark to write heat flux through the boundaries.
Solid Density : Mark to write solid density field in the results file.
Species Concentration : Mark to write species concentration field in the results file.
Phi Variable : Mark to write phi variables field in the results file.
Fluid Function #1 : Mark to write the function field (only evaluated in fluid domain) in the results file. The function field is written in IS units in the analysis group USERDEF. If this file is marked, two new field will be available.
Name : Name of the function. The corresponding field is identified with this name in the postprocessing part.
Function : Insert the fluid function to be evaluated and written. See Function Syntax section for further information.
Fluid Function #2 : Mark to write the function field (only evaluated in fluid domain) in the results file. The function field is written in IS units in the analysis group USERDEF. If this file is marked, two new field will be available.
Name : Name of the function. The corresponding field is identified with this name in the postprocessing part.
Function : Insert the fluid function to be evaluated and written. See Function Syntax section for further information.
Fluid Function #3 : Mark to write the function field (only evaluated in fluid domain) in the results file. The function field is written in IS units in the analysis group USERDEF. If this file is marked, two new field will be available.
Name : Name of the function. The corresponding field is identified with this name in the postprocessing part.
Function : Insert the fluid function to be evaluated and written. See Function Syntax section for further information.
Solid Function #1 : Mark to write the function field (only evaluated in solid domain) in the results file. The function field is written in IS units in the analysis group USERDEF. If this file is marked, two new field will be available.
Name : Name of the function. The corresponding field is identified with this name in the postprocessing part.
Function : Insert the fluid function to be evaluated and written. See Function Syntax section for further information.
Solid Function #2 : Mark to write the function field (only evaluated in solid domain) in the results file. The function field is written in IS units in the analysis group USERDEF. If this file is marked, two new field will be available.
Name : Name of the function. The corresponding field is identified with this name in the postprocessing part.
Function : Insert the fluid function to be evaluated and written. See Function Syntax section for further information.
Solid Function #3 : Mark to write the function field (only evaluated in solid domain) in the results file. The function field is written in IS units in the analysis group USERDEF. If this file is marked, two new field will be available.
Name : Name of the function. The corresponding field is identified with this name in the postprocessing part.
Function : Insert the fluid function to be evaluated and written. See Function Syntax section for further information.
Wave Elevation : Mark to write wave elevation field in the results file.
Wave Elevation Vector : Mark to write wave elevation vector field in the results file.
This group of data refers to all the information required to define the integration scheme and solver data of the problem/s to be analysed in the fluid domain.
Flow Solver Model : Flow solver model used in the fluid domain. Available options are Incompressible or PrCompressible (using a compressible algorithm based on pressure variable).
Remarks:
Incompressible model is adequate for problems with Mach number below 0.5, using the fully Incompressible or SlightlyIncompressible algorithm. See Materials section for further information.
Time Integration : Time integration scheme used in the solution process of the fluid problem:
Backward Euler : Implicit 1st order scheme.
Crank Nicolson : Implicit 2nd order scheme.
StabTauV MinRatio : Minimum admissible ratio (τ/dt, being dt the time increment) for the stabilisation parameter τ of the velocity solver. It will be also used for temperature and advection of species problems.
Remarks:
Advection stabilisation term is proportional to the parameter τ. In most of the cases, the minimum value of this parameter should not be fixed (i.e. τ/dt = 0.0), otherwise oscillations may appear.
StabTauP MinRatio : Minimum admissible ratio (τ/dt, being dt the time increment) for the stabilisation parameter τ of the pressure solver.
Remarks:
Advection stabilisation term is proportional to the parameter τ. In some cases with very small elements close to the wall, a value greater than 0.0 is required, in order to stabilise the pressure solution.
Solver NonSymmetric : Solver type used in the solution of the non-symmetric linear systems of equations.
BiConjugateGradient : Biconjugate gradient solver.
StabBiConjugateGradient : Stabilised biconjugate gradient solver.
GMRes : Generalised minimum residual solver.
SquaredConjugateGradient : Squared conjugate gradient solver.
Explicit : Jacobi type solver.
Tolerance : Tolerance used in the solution of the non-symmetric linear systems of equations (see Solver NonSymmetric ). A value smaller than 1.0·10-6 is recommended.
Max. Iterations : Maximum number of iterations of the non-symmetric linear systems of equations (see Solver NonSymmetric ).
Preconditioner : Preconditioner used in the solution of the non-symmetric linear systems of equations (see Solver NonSymmetric ).
Remarks:
In some cases using elements with high aspect ratio the diagonal preconditioner may work better than others.
Krilov sp. dimension : Dimension of internal direct solver used in GMRes solver (see Solver NonSymmetric ). A value greater than 20 is recommended.
Solver Symmetric : Solver type used in the solution of the symmetric linear systems of equations.
BiConjugateGradient : Biconjugate gradient solver.
StabBiConjugateGradient : Stabilised biconjugate gradient solver.
GMRes : Generalised minimum residual solver.
SquaredConjugateGradient : Squared conjugate gradient solver.
Explicit : Jacobi type solver.
Tolerance : Tolerance used in the solution of the symmetric linear systems of equations (see Solver Symmetric ). A value smaller than 1.0·10-6 is recommended.
Max. Iterations : Maximum number of iterations of the symmetric linear systems of equations (see Solver Symmetric ).
Preconditioner : Preconditioner used in the solution of the symmetric linear systems of equations (see Solver Symmetric ).
Remarks:
In some cases using elements with high aspect ratio the diagonal preconditioner may work better than others.
Krilov sp. dimension : Dimension of internal direct solver used in GMRes solver (see Solver Symmetric ). A value greater than 20 is recommended.
Advection Norm : Euclidean convergence norm of the velocity, used for recalculating or not advective terms. A value smaller than 1.0·10-5 is recommended.
Steady State Norm : Euclidean norm used to detect the steady state. If each variable increment is smaller than this norm, the problem is stopped and results are written to the disk.
Increment Control : This option activates a control that limits the maximum admisible increment of the variables for every iteration. The limit is taken as ratio of the convergence norm of the variable. Select None to switch this control off.
This group of data refers to all the information required to define the integration scheme and solver data of the problem/s to be analysed in the solid domain.
Flow Solver Model : Flow solver model used in the fluid domain. Available options are Incompressible or PrCompressible (using a compressible algorithm based on pressure variable).
Remarks:
Incompressible model is adequate for problems with Mach number below 0.5, using the fully Incompressible or SlightlyIncompressible algorithm. See Materials section for further information.
Time Integration : Time integration scheme used in the solution process of the solid problem:
Backward Euler : Implicit 1st order scheme.
Crank Nicolson : Implicit 2nd order scheme.
Solver NonSymmetric : Solver type used in the solution of the symmetric linear systems of equations.
BiConjugateGradient : Biconjugate gradient solver.
StabBiConjugateGradient : Stabilised biconjugate gradient solver.
GMRes : Generalised minimum residual solver.
SquaredConjugateGradient : Squared conjugate gradient solver.
Explicit : Jacobi type solver.
Tolerance : Tolerance used in the solution of the symmetric linear systems of equations (see Solver Symmetric ). A value smaller than 1.0·10-6 is recommended.
Max. Iterations : Maximum number of iterations of the symmetric linear systems of equations (see Solver Symmetric ).
Preconditioner : Preconditioner used in the solution of the symmetric linear systems of equations (see Solver Symmetric ).
Remarks:
In some cases using elements with high aspect ratio the diagonal preconditioner may work better than others.
Krilov sp. dimension : Dimension of internal direct solver used in GMRes solver (see Solver Symmetric ). A value greater than 20 is recommended.
Steady State Norm : Norm used to detect the steady state. A value smaller than 1.0·10-5 is recommended.
Increment Control : This option activates a control that limits the maximum admisible increment of the variables for every iteration. The limit is taken as ratio of the convergence norm of the variable. Select None to switch this control off.
Floatability by Density : If selected, density variations generate a floatability phenomenon that otherwise is ignored.
Use Total Pressure : Mark if you want to use total pressure (including fluid-static term) as internal variable in the solution of the fluid flow problem.
Remarks:
In most of the cases the solution of the fluid problem without fluid-static term is the most accurate one.
If this option is selected, please check the correctness of the pressure boundary conditions. These should take into account the fluid-static pressure term.
Operating Pressure : Reference pressure for compressible solvers.
Pressure reference location : Mark if you want to define the origin of the fluid-static pressure term.
Pressure Origin : Coordinates of the total pressure origin.
Xplane Symmetry in Fluid : Mark if you want to define symmetry planes in the fluid problem, perpendicular to OX axis.
Xplane Symmetry Position : Position of the symmetry planes in the fluid problem, perpendicular to OX axis, given in the units of the geometry.
Yplane Symmetry in Fluid : Mark if you want to define symmetry planes in the fluid problem, perpendicular to OY axis.
Yplane Symmetry Position : Position of the symmetry planes in the fluid problem, perpendicular to OY axis, given in the units of the geometry.
Zplane Symmetry in Fluid : Mark if you want to define symmetry planes in the fluid problem, perpendicular to OZ axis.
Zplane Symmetry Position : Position of the symmetry planes in the fluid problem, perpendicular to OZ axis, given in the units of the geometry.
Law of the wall type : Law of the wall implementation to be used. DepTau implementation corrects the stress to be imposed as boundary condition on the wall, depending of the data given by the user and the law of the wall stress. If FixTau is selected, Tdyn will impose the law of the wall stress as boundary condition (as done in Tdyn 3.5 and below).
Remarks:
DepTau scheme is normally more accurate for small or large y+ values, while FixTau scheme should be used for intermediate values.
Law of the wall vfor : If On , when possible law of the wall data will be used to calculate viscous forces. If Off , viscous forces will be evaluated using velocity field.
Tcl extension : If the checkbox is selected, the Tcl extension of Tdyn is activated. The entry may indicate a tcl script to be interpreted during Tdyn execution. The Tcl script can define any of the stardard Tdyn Tcl functions. See section Tdyn Tcl Extension for further information about Tcl extension of Tdyn.