Tdyn reference manual


Boundaries

Boundaries are groups of geometrical or mesh entities with common boundary conditions and other data. These boundaries identify :

▪      External boundary of a body or a part of a body in a fluid or solid.

▪      Any external boundary of the fluid or solid with prescribed heat flux.

▪      Any external boundary of the fluid or solid with prescribed concentration flux of species.

▪      Any external boundary of the fluid or solid with prescribed flux of a variable.

▪      A free surface for naval problems.

Boundaries can be assigned to surfaces (Tdyn3D) or lines (Tdyn2D) or boundary meshes. The user may create new boundaries derived from the existing ones and assign them as well.

To create a new Boundary, press the New Boundary button in the Boundary window, write a new name and change some of its properties. By pressing Accept, a new boundary is created taking an existing one as a base Boundary, which means that the new boundary will have the same fields as the base one. All new values for the fields can be entered when defining the new boundary. It is also possible to redefine existing boundaries by entering new values directly in the fields.

Remarks:

If a mesh has already been generated and new boundaries are assigned to the geometry or some of the existing ones are removed, it is necessary to mesh again.

Fluid Body

Fluid Body boundaries are groups of boundary conditions, geometrical properties and other data, that identify a body as a boundary of a fluid in the analysis. These properties can be assigned to lines (2D) or surfaces (3D) or boundary meshes.

Remarks:

If any entity is defined as a Fluid Body the graphs of the reaction forces on the fluid will be available in the post-process of Tdyn.

If any entity is defined as a Fluid Body and any movement is enabled, the graphs of this movement will be available in the post-process of Tdyn.

In order to transfer Fluid Body data to the mesh, Meshing Criteria must be fixed to Yes in the corresponding geometrical entities. Note that this action is automatically done by Tdyn in most of the cases.

Options available in module RANSOL

BoundType: Type of the wall boundary. Several options are available:

InvisWall: Impose the slipping boundary condition (i.e. wall normal velocity component will be zero).

V_fixWall: Impose the null velocity condition on the boundary (i.e. velocity on the wall will be zero).

None_Wall: No conditions will be applied to the boundary.

RoughWall: Law of the wall condition, taking wall roughness into account, is applied at the wall distance δ. See Near wall-modelling chapter below. The fluid stress (traction) given by the law of the wall at a wall distance δ will be applied as boundary condition in the fluid solver. The wall distance must be inserted in the field Delta (see below).

DeltaWall: Extended law of the wall condition is applied on the boundary at the wall distance δ. See Near wall-modelling chapter below. The fluid stress (traction) given by the law of the wall at a wall distance δ will be applied as boundary condition in the fluid solver. The wall distance must be inserted in the field Delta (see below).

YplusWall: Extended Law of the wall condition is applied on the boundary at the non-dimensional wall distance y+. See Near wall-modelling chapter below. The fluid stress (traction) given by the law of the wall at a non-dimensional wall distance y+ will be applied as boundary condition in the fluid solver. The non-dimensional wall distance must be inserted in the field Yplus (see below).

Cw_U2Wall: A traction given by CW·V2, where CW is a constant and V the fluid velocity, is imposed on the boundary. The constant CW must be inserted in the field Cw (see below).

ITTC Wall: Extended Law of the wall condition is applied on the boundary at the non-dimensional wall distance y+. The fluid stress (traction) given by the law of the wall at a non-dimensional wall distance y+ will be applied as boundary condition in the fluid solver. This traction  is corrected according to the ITTC 57 friction law. The non-dimensional wall distance must be inserted in the field Yplus (see below).

User Wall: Law of the wall formulation that can be defined by the user. It requires explicit formulation of the wall traction (see below FTau Field), eddy kinetic energy (see below KEnr Field) and the turbulence length scale (see below ELen Field).

OutFBound: The Tdyn implementation of a free boundary condition is applied on the boundary.

Yplus:   If YplusWall is selected, wall law assumption is taken up to the non-dimensional wall distance y+ given here. The fluid stress (traction) given by the law of the wall will be then applied as a boundary condition in the fluid solver. See Near wall-modelling chapter below.

Delta:  If DeltaWall is selected, wall law assumption is taken up to the dimensional wall distance δ specified here. The fluid stress (traction) given by the law of the wall will be then applied as a boundary condition in the fluid solver. See Near wall-modelling chapter below.

Delta Units: Units of the dimensional wall distance δ given in the previous field.

Roughness: Roughness of the wall (only used if BoundType \ RoughWall is selected).

Roughness Units: Units of the dimensional wall distance δ given in the previous field.

Cw: Constant used in the definition of BoundType \ Cw_U2Wall.

FTau Field: Field of wall traction used in the definition of BoundType \ User Wall. It should be a explicit function of the variables used in Tdyn (see Function Syntax section for further information). It will be evaluated in the internal units given in Data > Units Data.

KEnr Field: Field of eddy kinetic energy used in the definition of BoundType \ User Wall. It should be a explicit function of the variables used in Tdyn (see Function Syntax section for further information). It will be evaluated in the internal units given in Data > Units Data.

ELen Field: Field of turbulence length scale used in the definition of BoundType \ User Wall. It should be a explicit function of the variables used in Tdyn (see Function Syntax section for further information). It will be evaluated in the internal units given in Data > Units Data.

Sharp Angle: Any applied slipping or law of the wall boundary condition on the velocity field will be corrected if any internal angle of this Fluid Body geometry will be smaller than the one inserted here (see Figure 12). This condition should be used for automatic correction of boundary conditions, in those complex geometries with trailing edges, where the Fluid Body normal vector is undefined. Units of the sharp angle angle field may be defined in Data > Units data > GENERAL > Boundary Angle Units.

Figure 12. Example of application of the Sharp Angle option.

Line Fix Angle: Fix Velocity Direction boundary conditionwill be automatically applied as boundary condition if an external angle of this Fluid Body geometry is smaller than the one inserted here (see Figure 13). This condition should be used to automatically impose Fix Velocity Direction boundary conditions, in those complex geometries with edges or significant dihedral angles, where boundary conditions imposition by hand, may take too much time. Units of the line fix angle field may be defined in Data > Units data > GENERAL > Boundary Angle Units.

Remarks:

In Tdyn 2D a null velocity is imposed (instead of FixVelocity Direction condition) if an external angle of a Fluid Body is smaller than the one inserted here.

Figure 13. Example of the places where the Line Fix Angle option could be useful.

SternC Angle: A control for stern of bodies (in the transpiration problem available in the NAVAL module of Tdyn) is carried out. This control will be applied in those points of the floating line of the body, where the angle between the normal and the velocity is greater that the value inserted here. See Stern flow modelling in transpiration problem section. Units of the sternc angle field may be defined in Data > Units data > GENERAL > Boundary Angle Units.

 

Remarks:

This option is only available in the NAVAL module.

Options available in module HEATRANS

Heat Flux: Heat flow (power) entering to the domain through this Fluid Body. It may be a constant or a function. See Function Syntax section for further information. Units of the heat flux field may be defined in the menu next to this entry. It is possible to define additional units by entering new dimensionally correct units in the box (see Units Syntax section for further information).

Reactive Heat Flux: Factor of the reactive term of the heat flow (power) entering to the domain through this Fluid Body. The value here inserted will be multiplied by the current temperature to obtain the heat flow. It may be a constant or a function. See Function Syntax section for further information. Units of the reactive heat flux field may be defined in the menu next to this entry. It is possible to define additional units by entering new dimensionally correct units in the box (see Units Syntax section for further information).

Remarks:

Convection heat tranfer may be simulated by inserting the function q + h*(tm-to) in the field Heat Flux, being q a defined heat flow, h the transmission coefficient and to the external temperature. However it is recommended to split this flow in two terms, constant flow q +h*to that should be inserted in the Heat Flow field and temperature dependant term h that should be entered in Reactive Heat Flux field.

Note that positive values means heat flow entering in the domain.

Options available in module ADVECT

ADVECT label of Fluid Body window is splitted in two frames. Left frame shows a list of the defined species and the currently selected one. To select a different species, just click on its name. Right frame shows the entries presented next.

Flux Spc: Flow of the species entering to the domain through this Fluid Body. It may be a constant or a function. See Function Syntax section for further information. Units of the flux spc field may be defined in the menu next to this entry. It is possible to define additional units by entering new dimensionally correct units in the box (see Units Syntax section for further information).

Reactive Flux Spc: Factor of the reactive term of the flow of the species entering to the domain through this Fluid Body. The value here inserted will be multiplied by the current species concentratio to obtain the heat flow. It may be a constant or a function. See Function Syntax section for further information. Units of the reactive flux spc field may be defined in the menu next to this entry. It is possible to define additional units by entering new dimensionally correct units in the box (see Units Syntax section for further information).

Remarks:

Entering flow of species of the form h·sp1 should be inserted in the Reactive Flux Spc field as h.

Note that positive values means flow entering in the domain.

Options available in module URSOLVER

URSOLVER label of Fluid Body window is splitted in two frames. Left frame shows a list of the defined variables and the currently selected one. To select a different variable, just click on its name. Right frame shows the entries presented next.

Flux Phi: Flow of the variable entering to the domain through this Fluid Body. It may be a constant or a function. See Function Syntax section for further information. Units of the flux phi field may be defined in the menu next to this entry. It is possible to define additional units by entering new dimensionally correct units in the box (see Units Syntax section for further information).

Reactive Flux Phi: Factor of the reactive term of the flow of the species entering to the domain through this Fluid Body. The value here inserted will be multiplied by the current variable concentratio to obtain the heat flow. It may be a constant or a function. See Function Syntax section for further information. Units of the reactive flux phi field may be defined in the menu next to this entry. It is possible to define additional units by entering new dimensionally correct units in the box (see Units Syntax section for further information).

Remarks:

Entering flow of the variable of the form h·ph1 should be inserted in the Reactive Flux Phi field as h.

Note that positive values means flow entering in the domain.

Options available in module ALEMESH

Body Mass: Mass of the body. Units of the mass field may be defined in the menu next to this entry. It is possible to define additional units by entering new dimensionally correct units in the box (see Units Syntax section for further information).

Remarks:

If the check box next to the Body Mass entry is selected, mass of the body will be estimated by Tdyn, based on a initial forces equilibrium.

Body Mass entry will be always available for the rest of the modules of Tdyn.

Center of Gravity: Vector giving the center of gravity of the body. Units of the center of gravity may be defined in Data > Units data > GEOMETRY > Geometry Units.

Remarks:

Center of Gravity entry will be always available for the rest of the modules of Tdyn.

Center of Gravity may be defined by a time dependant function.

Radi-us/-i of Gyration: Vector giving the radii of gyration of the body. Units of the radii of gyration may be defined in Data > Units data > GEOMETRY > Geometry Units.

Displacement Options: For every displacement degree of freedom there exists three possible options:

Off: the corresponding degree of freedom is disabled (movement is not allowed).

On: the corresponding degree of freedom is enables (movement is allowed). If the value inserted in the corresponding Displacement Values field is different from cero for t = 0, this value will be used to define an initial movement of the body.

Fix: the corresponding degree of freedom is fixed to the value given by the Displacement Values field (movement is prescribed).

Displacement Values: For every displacement degree of freedom, this vector gives the total displacement of the body. The corresponding fields will only be available if the Displacement Options field is selected as Fix. Units of the displacement values vector  may be defined in Data > Units data > GEOMETRY > Geometry Units.

Rotation Options: For every rotational degree of freedom there exists three possible options:

Off: the corresponding degree of freedom is disabled (rotation is not allowed).

On: the corresponding degree of freedom is enables (rotation is allowed). If the value inserted in the corresponding Rotation Values field is different from cero for t = 0, this value will be used to define an initial movement of the body.

Fix: the corresponding degree of freedom is fixed to the value given by the Rotation Values field (rotation is prescribed).

Rotation Values: For every rotational degree of freedom, this vector gives the total rotation of the body. The corresponding fields will only be available if the Rotation Options field is selected as Fix. Units of the rotation values vector may be defined in Data > Units data > GENERAL > Boundary Angle Units.

Springs: This list give the spring constants (displacement-KD and rotation-KR) and the origin (Fix) and End (its initial position) of the springs linked to the body (end point of the spring follows the movement of the body). Units of the spring constants KD and KR are given in the fields below.


Solid Body

Solid Body boundaries are groups of boundary conditions, geometrical properties and other data, that identify a boundary of a solid in the analysis. These properties can be assigned to lines (Tdyn2D) or surfaces (Tdyn3D) or boundary meshes.

Remarks:

If any entity is defined as a Solid Body the graphs of the reaction forces on the fluid will be available in the post-process of Tdyn.

If any entity is defined as a Solid Body and any movement is enabled, the graphs of this movement will be available in the post-process of Tdyn.

In order to transfer Solid Body data to the mesh, Meshing Criteria must be fixed to Yes in the corresponding geometrical entities. Note that this action is automatically done by Tdyn in most of the cases.

Options available in module RANSOL

BoundType: Type of the wall boundary. Several options are available:

InvisWall: Impose the slipping boundary condition (i.e. wall normal velocity component will be zero).

V_fixWall: Impose the null velocity condition on the boundary (i.e. velocity on the wall will be zero).

None_Wall: No conditions will be applied to the boundary.

User Wall: Law of the wall formulation that can be defined by the user. It requires explicit formulation of the wall traction (see below FTau Field), eddy kinetic energy (see below KEnr Field) and the turbulence length scale (see below ELen Field).

OutFBound: The Tdyn implementation of a free boundary condition is applied on the boundary.

FTau Field: Field of wall traction used in the definition of BoundType \ User Wall. It should be a explicit function of the variables used in Tdyn (see Function Syntax section for further information). It will be evaluated in the internal units given in Data > Units Data.

KEnr Field: Field of eddy kinetic energy used in the definition of BoundType \ User Wall. It should be a explicit function of the variables used in Tdyn (see Function Syntax section for further information). It will be evaluated in the internal units given in Data > Units Data.

ELen Field: Field of turbulence length scale used in the definition of BoundType \ User Wall. It should be a explicit function of the variables used in Tdyn (see Function Syntax section for further information). It will be evaluated in the internal units given in Data > Units Data.

Sharp Angle: Any applied slipping condition on the velocity field will be corrected if any internal angle of this Solid Body geometry will be smaller than the one inserted here (see Figure 12). This condition should be used for automatic correction of boundary conditions, in those complex geometries with trailing edges, where the Solid Body normal vector is undefined. Units of the sharp angle field may be defined in Data > Units data > GENERAL > Boundary Angle Units.

Line Fix Angle: Fix Velocity Direction boundary condition will be automatically applied as boundary condition if an external angle of this Solid Body geometry is smaller than the one inserted here (see Figure 13). This condition should be used to automatically impose FixVelocity Direction boundary conditions, in those complex geometries with edges or significant dihedral angles, where boundary conditions imposition by hand, may take too much time. Units of the line fix angle field may be defined in Data > Units data > GENERAL > Boundary Angle Units.

Remarks:

In Tdyn 2D a null velocity is imposed (instead of FixVelocity Direction condition) if an external angle of a Solid Body is smaller than the one inserted here.

SternC Angle: A control for stern of bodies (in the transpiration problem available in the NAVAL module of Tdyn) is carried out. This control will be applied in those points of the floating line of the body, where the angle between the normal and the velocity is greater that the value inserted here. See Stern flow modelling in transpiration problem section. Units of the sternc angle field may be defined in Data > Units data > GENERAL > Boundary Angle Units.

 

Remarks:

This option is only available in the NAVAL module.

Options available in module HEATRANS

Heat Flux: Heat flow (power) entering to the domain through this Solid Body. It may be a constant or a function. See Function Syntax section for further information. Units of the heat flux field may be defined in the menu next to this entry. It is possible to define additional units by entering new dimensionally correct units in the box (see Units Syntax section for further information).

Reactive Heat Flux: Factor of the reactive term of the heat flow (power) entering to the domain through this Solid Body. The value here inserted will be multiplied by the current temperature to obtain the heat flow. It may be a constant or a function. See Function Syntax section for further information. Units of the reactive heat flux field may be defined in the menu next to this entry. It is possible to define additional units by entering new dimensionally correct units in the box (see Units Syntax section for further information).

Remarks:

Convection heat tranfer may be simulated by inserting the function q + h*(tm-to) in the field Heat Flux, being q a defined heat flow, h the transmission coefficient and to the external temperature. However it is recommended to split this flow in two terms, constant flow q +h*to that should be inserted in the Heat Flow field and temperature dependant term h that should be entered in Reactive Heat Flux field.

Note that positive values means heat flow entering in the domain.

Options available in module ADVECT

ADVECT label of Solid Body window is splitted in two frames. Left frame shows a list of the defined species and the currently selected one. To select a different species, just click on its name. Right frame shows the entries presented next.

Flux Spc: Flow of the species entering to the domain through this Solid Body. It may be a constant or a function. See Function Syntax section for further information. Units of the flux spc field may be defined in the menu next to this entry. It is possible to define additional units by entering new dimensionally correct units in the box (see Units Syntax section for further information).

Reactive Flux Spc: Factor of the reactive term of the flow of the species entering to the domain through this Solid Body. The value here inserted will be multiplied by the current species concentratio to obtain the heat flow. It may be a constant or a function. See Function Syntax section for further information. Units of the reactive flux spc field may be defined in the menu next to this entry. It is possible to define additional units by entering new dimensionally correct units in the box (see Units Syntax section for further information).

Remarks:

Entering flow of species of the form h·sp1 should be inserted in the Reactive Flux Spc field as h.

Note that positive values means flow entering in the domain.

Options available in module URSOLVER

URSOLVER label of Solid Body window is splitted in two frames. Left frame shows a list of the defined variables and the currently selected one. To select a different variable, just click on its name. Right frame shows the entries presented next.

Flux Phi: Flow of the variable entering to the domain through this Solid Body. It may be a constant or a function. See Function Syntax section for further information. Units of the flux phi field may be defined in the menu next to this entry. It is possible to define additional units by entering new dimensionally correct units in the box (see Units Syntax section for further information).

Reactive Flux Phi: Factor of the reactive term of the flow of the species entering to the domain through this Solid Body. The value here inserted will be multiplied by the current variable concentratio to obtain the heat flow. It may be a constant or a function. See Function Syntax section for further information. Units of the reactive flux phi field may be defined in the menu next to this entry. It is possible to define additional units by entering new dimensionally correct units in the box (see Units Syntax section for further information).

Remarks:

Entering flow of the variable of the form h·ph1 should be inserted in the Reactive Flux Phi field as h.

Note that positive values means flow entering in the domain.

Options available in module ALEMESH

Body Mass: Mass of the body. Units of the mass field may be defined in the menu next to this entry. It is possible to define additional units by entering new dimensionally correct units in the box (see Units Syntax section for further information).

Remarks:

If the check box next to the Body Mass entry is selected, mass of the body will be estimated by Tdyn, based on a initial forces equilibrium.

Body Mass entry will be always available for the rest of the modules of Tdyn.

Center of Gravity: Vector giving the center of gravity of the body. Units of the center of gravity may be defined in Data > Units data > GEOMETRY > Geometry Units.

Remarks:

Center of Gravity entry will be always available for the rest of the modules of Tdyn.

Radi-us/-i of Gyration: Vector giving the radii of gyration of the body. Units of the radii of gyration may be defined in Data > Units data > GEOMETRY > Geometry Units.

Displacement Options: For every displacement degree of freedom there exists three possible options:

Off: the corresponding degree of freedom is disabled (movement is not allowed).

On: the corresponding degree of freedom is enables (rotation is allowed). If the value inserted in the corresponding Displacement Values field is different from cero for t = 0, this value will be used to define an initial movement of the body.

Fix: the corresponding degree of freedom is fixed to the value given by the Displacement Values field (movement is prescribed).

Displacement Values: For every displacement degree of freedom, this vector gives the total displacement of the body. The corresponding fields will only be available if the Displacement Options field is selected as Fix. Units of the displacement values vector  may be defined in Data > Units data > GEOMETRY > Geometry Units.

Rotation Options: For every rotational degree of freedom there exists three possible options:

Off: the corresponding degree of freedom is disabled (rotation is not allowed).

On: the corresponding degree of freedom is enables (rotation is allowed). If the value inserted in the corresponding Rotation Values field is different from cero for t = 0, this value will be used to define an initial movement of the body.

Fix: the corresponding degree of freedom is fixed to the value given by the Rotation Values field (rotation is prescribed).

Rotation Values: For every rotational degree of freedom, this vector gives the total rotation of the body. The corresponding fields will only be available if the Rotation Options field is selected as Fix. Units of the rotation values vector may be defined in Data > Units data > GENERAL > Boundary Angle Units.

Springs: This list give the spring constants (displacement-KD and rotation-KR) and the origin (Fix) and End (its initial position) of the springs linked to the body (end point of the spring follows the movement of the body). Units of the spring constants KD and KR are given in the fields below.

Free Surface

Free Surface boundaries are groups of boundary conditions, and other data, that identify a free surface boundary of a fluid in the analysis. These properties can be assigned to surfaces (3D).

Remarks:

Free Surface boundary is only available in NAVAL module of Tdyn 3D.

In order to transfer Free Surface data to the mesh, Meshing Criteria must be fixed to Yes in the corresponding geometrical entities. Note that this action is automatically done by Tdyn in most of the cases.

Options available in module NAVAL

Time Integration: Time integration scheme used in the solution process of the free surface problem. The following options are available:

Adams_Bashforth_2: Explicit 2nd order Adams Bashforth scheme.

Stabilised_FIC: Time stabilised FIC scheme.

Backward_Euler: Implicit 1st order Backward Euler scheme.

Forward_Euler: Explicit 1st order Forward Euler scheme.

Crank_Nicolson: Implicit 2nd order Crank-Nicolson scheme.

Advect_Stabilisation: The order of the FIC advection stabilisation term in the free surface equation. Two options are available 4th_Order and 2nd_Order.

Remarks:

The 4th order term increases the accuracy of the solution and is recommended in most of the cases, but in some problems may appear instabilities.

StabTau_MinRatio: Minimum admissible ratio (τ/dt, being dt the time increment) for the stabilisation parameter τ.

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.

Length: Characteristic length of the free surface problem (i.e. length of the Fluid Body).

Length Units: Units for the characteristic length of the free surface problem.

Damping length: Relative damping length (Damping Length x Length) to be used in this free surface (see Figure 14). In some cases it is necessary to damp the wave elevation in order not to find bouncing effects in the boundaries.

Figure 14. Damping area in the free surface solution.

Damping factor: Factor that controls the damping effect.

Time factor: Time integration security factor to be used in the explicit integration (i.e. Adams_Bashforth_2, Stabilised_FIC and Forward_Euler schemes) of this free surface.

Step factor: Time step ratio between free surface and fluid solver. It is possible to accelerate convergence by increasing this ratio, but may cause unstability in the integration scheme. If chosen Time Increment is too high, reduce this value to achieve convergence.

Remarks:

Note that solutions with Step factor != 1 may only be realistic in the free surface steady state.