tdynreference manual


Boundaries

Boundaries are groups of boundary conditions, geometrical properties and other data, that identify a boundary of the analysis.

Remarks:

Most of the boundary conditions must be defined using the standard condition windows (see Conditions chapter). However, some complex boundary conditions are applied easier and almost automatically by using the Boundaries options.

For any problem that requires definition of boundaries, there is a basic database that can be used to define the problem. The user can also create new boundaries derived from the existing ones and assign them as well.

To create a new boundary, press the New Boundaries button in the Boundaries window, write the boundary name and modify 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 values of new field can be entered. It is also possible to redefine existing Boundaries by entering new values directly into their fields.

Remarks:

If a mesh has already been generated, for any change in the assigned materials, it is necessary to mesh again or assign the Boundaries directly to the mesh.


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).

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.

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).

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 Cw_U2Wall \ BoundType.

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 5). 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. 

Figure 5. Example of application of the Sharp Angle option.

Line Fix Angle: Velocity Line will be automatically applied as boundary condition if an external angle of this Fluid Body geometry is smaller than the one inserted here (see Figure 6). This condition should be used to automatically impose Velocity Line boundary conditions, in those complex geometries with edges or significant dihedral angles, where boundary conditions imposition by hand, may take too much time. 

Remarks:

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

Figure 6. 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.

 

Remarks:

This option is only available in the NAVAL module.

Angle Units: Units of the angular variables inserted in the previous fields.

Options available in module HEATRANS

Heat Flux: Diffusion heat power (Q) entering to the domain through this Fluid Body. It may be a constant or a function. See Function Syntax section for further information.

Remarks:

Convection heat tranfer may be simulated by defining the function q + h*(tm-to), being q a defined heat flow, h the transmission coefficient and, to the external temperature.

Units of Heat Flux are defined in the Units window, see Options available in Boundary Units tag for further information.

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

Fluid Boundary

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

Remarks:

Note that Fluid Boundary is nothing but a simplified version of a Fluid Body.

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

In order to transfer Fluid Boundary 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 on the boundary.

Sharp Angle: Any applied slipping or Law of the Wall boundary condition on the velocity field will be corrected if any of the internal angles of the Fluid Boundary geometry is smaller than the one inserted here (see Figure 5). This condition should be used to automatically correct the boundary conditions, in those complex geometries with trailing edges, where the Fluid Boundary normal vector is undefined. 

Line Fix Angle: Velocity Line will be automatically applied as boundary condition if an external angle of this Fluid Boundary geometry is smaller than the one inserted here (see Figure 6). This condition should be used to automatically impose Velocity Line boundary conditions, in those complex geometries with edges or significant dihedral angles, where boundary conditions imposition by hand, may take too much time. 

Remarks:

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

Angle Units: Units of the angular variables inserted in the previous fields.

Options available in module HEATRANS

Heat Flux: Diffusion heat power (Q) entering to the domain through this Fluid Body. It may be a constant or a function. See Function Syntax section for further information.

Remarks:

Convection heat tranfer may be simulated by defining the function q + h*(tm-to), being q a defined heat flow, h the transmission coefficient and, to the external temperature.

Units of Heat Flux are defined in the Units window, see Options available in Boundary Units tag for further information.

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

Solid Boundary

Solid Boundary 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 (2D) or surfaces (3D).

Remarks:

In order to transfer Solid Boundary 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 HEATRANS

Heat Flux: Diffusion heat power (Q) entering to the domain through this Fluid Body. It may be a constant or a function. See Function Syntax section for further information.

Remarks:

Convection heat tranfer may be simulated by defining the function q + h*(tm-to), being q a defined heat flow, h the transmission coefficient and, to the external temperature.

Units of Heat Flux are defined in the Units window, see Options available in Boundary Units tag for further information.

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

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 7). In some cases it is necessary to damp the wave elevation in order not to find bouncing effects in the boundaries.

Figure 7. 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.