GLS3D Interface

US Army Corps of Engineers (USACE)
modeling software for Navier-Stokes problems  

T

(Return)

The interface writes the command deck or batch file according to the GLS3D specifications, using ADH format. The GLS3D batch file created with the ICEM CFD/CAE translator outputs two files:

• Geometry file:                              project_name.3dm
• Boundary Conditions file:        project_name.bc

Creating the GLS3D Input Files

The translator writes the GLS3D batch file using the following files:

• unstructured domain file generated by Tetra Mesher
• boundary condition file
• parameter file (gls3d.params)

To create the GLS3D input file, select the following menu entries from the ICEM CFD/CAE manager:

• output menu; select translator GLS3D
• output menu; GLS3D input
• specify options for the GLS3D interface:
• select an existing unstructured domain file (default is cut_domain.1)
• give the name of the boundary condition file (default is configuration/parts_mesh/mesh/family_boco)
• give the name of the GLS3D input file (default is configuration/parts_mesh/transfer/gls3d)
• specify a scaling factor, is applicable.
• specify GLS3D parameters:

            - Operation Parameters
            - Iteration Parameters
            - Material Property
            - Time Control

After successful execution of the translator, the GLS3D file is located in the directory "transfer".
 

Defining Parameters for GLS3D

All parameters appearing in the GLS3D input file may be defined within a Graphical User Interface (GUI) which is automatically executed when the GLS3D translator is ran. Each parameters group may be turned ON or OFF using the check-button on the left side column. When a parameter group is ON, then its values may be edited by clicking on the button "Edit".

The four parameters groups and their contents are:

1. Operation Parameters:

Select if a Navier-Stokes problem (default is Navier-Stokes)

Enter Incremental memory    (defaut is 1)

Enter Transport quantities (defaut is 0)

        - if Navier-Stokes selected, Transport quantities must be zero.
           If not, it is automatically reset to zero, and a message is printed.

Enter Time step weighting (default is 1.0)

Enter number of Blocks per processor (default is 1)

Select Pre-conditioner    (default is No pre-conditioner)

2. Iteration Parameters:

Enter number of Non-linear iterations per time-step (default is 0)

Enter Tolerance for non-linear equations (defaut is 0.0)

Enter  Maximum number of linear iterations (defaut is 1)

Select to accept the non-linear solution  even if the tolerance is not satisfied (option 2)

Select to accept the linear solution  even if the tolerance is not satisfied (opion 2)

3. Material Property:

• Flow parameters:
• Enter viscosity (default is 0.0)
• Enter density (default is 1.94)
• Enter gravitational acceleration (default is 32.4)
• Reference Flow parameters:
• Enter reference viscosity (default is 0.0)
• Enter reference density (default is 1.94)
• Enter reference velocity (default is 0.0)
• Enter reference length (default is 0.0)
• Stabilization coefficients:
• Enter Galerkin least squares stabilization coeff. associated with the momentum equations (default is 0.0)
• Enter Galerkin least squares stabilization coeff. associated with the continuity equations (default is 0.0)
• Time Control:
• Enter solution starting time and ending time (default is 0.0)
• Enter time step size at solution starting time and ending time (default is 0.0)
• Enter "global" starting time and ending time (default is 0.0)
• Select adaptive time control to refine time steps from those specified above by the user.
• Select non adaptive time steps to refine time steps for stability puropose
• Enter times to output solution (default is 0.0).

        - If all output solution are 0.0, one is automatically set equal to the ending time.
 
 

Defining boundary conditions for GLS3D

The next sections describe how to define GLS3D commands using the Unspecified bound. cond. menu in MULCAD, the general bound. cond. menu in the DDN-Mesher Interface. In the mesh editor (MED), one just have to fill up the Output/Bound conds menu.
Please refer to the General Remarks section for more details.
 

Dirichlet External Pressure:

The pressure for this family is defined by an external program.

In the mesh editor Output/Bound conds menu, the family is automatically tag when selecting the BC type "Dirichlet External Pressure"
Otherwise, the  user defined variables:

    MULCAD      DDN-Mesher
    ------      ----------
    1.FLAG      1.string1       DEXT

Node card (NDS) will be written in project_name.bc for each node of this family.
 

Dirichlet Pressure:

In the mesh editor Output/Bound conds menu, the family is automatically tag when selecting the BC type "Dirichlet External Pressure"
Otherwise, the  user defined variables:

    MULCAD      DDN-Mesher
    ------      ----------
    1.FLAG      1.string1    DPRS     
    3.VALUE     4.real1      initial time t0
    4.X         5.real2      final time tf
    5.Y         6.real3      pressure at t0
    6.Z         7.real4      pressure at tf

Node card (NDS) will be written in project_name.bc for each node of this family.
 

Dirichlet Velocity:

In the mesh editor Output/Bound conds menu, the user defined the required bc value shown in the menu.
Otherwise, the  user defined variables:

    MULCAD      DDN-Mesher
    ------      ----------
    1.FLAG      1.string1    DVEL    
    3.VALUE     4.real1      initial time t0
    4.X         5.real2      final time tf
    5.Y         6.real3      x-velocity at t0    
    6.Z         7.real4      x-velocity at tf
    7.SCALE     8.real5      y-velocity at t0
    8.A         9.real6      y-velocity at tf    
    9.B        10.real7      z-velocity at t0
   10.C        11.real8      z-velocity at tf

Node card (NDS) will be written in project_name.bc for each node of this family.
 

NeumannVelocity:

In the mesh editor Output/Bound conds menu, the user defined the required bc value shown in the menu.
Otherwise, the  user defined variables:

    MULCAD      DDN-Mesher
    ------      ----------
    1.FLAG      1.string1    NVEL    
    3.VALUE     4.real1      initial time t0
    4.X         5.real2      final time tf
    5.Y         6.real3      outflow velocity at t0    
    6.Z         7.real4      outflow velocity at tf
    7.SCALE     8.real5      Darcy-Weisbach friction (drag)

Face card (FCS) will be written in project_name.bc for each node of this family.
 

Outflow:

It identify a face for which the flow is allowed to pass out of the domain.

In the mesh editor Output/Bound conds menu, the faces are automatically tag.
Otherwise, the  user defined variables:

    MULCAD      DDN-Mesher
    ------      ----------
    1.FLAG      1.string1    OVEL

Face card (FCS) will be written in project_name.bc for each node of this family.
 

Outflow External:

It identify  face for which the flow information is suplied by an external program.

In the mesh editor Output/Bound conds menu, the faces are automatically tag.
Otherwise, the  user defined variables:

    MULCAD      DDN-Mesher
    ------      ----------
    1.FLAG      1.string1    OEXT

Face card (FCS) will be written in project_name.bc for each node of this family.
 

Eddy Viscosity:

Material property applied to families

In the mesh editor Output/Bound conds menu, just fill up the boxeds with the required value.
Otherwise, the  user defined variables:

    MULCAD      DDN-Mesher
    ------      ----------
    1.FLAG      1.string1       MP
    3.VALUE     4.real1         Enter the value of Exx
    4.X         5.real2         Enter the value of Eyy
    5.Y         6.real3         Enter the value of Ezz    
    6.Z         7.real4         Enter the value of Exy
    7.SCALE     8.real5         Enter the value of Exz
    8.A         9.real6         Enter the value of Eyz
   12.A         2.string2       EV

Mesh Refinement:

In the mesh editor Output/Bound conds menu, just fill up the boxeds with the required value.
Otherwise, the  user defined variables:

    MULCAD      DDN-Mesher
    ------      ----------
    1.FLAG      1.string1       MP
    2.NR        3.integer       Enter the maximum level of refinement
    3.VALUE     4.real1         Enter the error tolerance for the refinement terms
    4.X         5.real2         Enter the error tolerance for unrefining elements
   12.A         2.string2       MESH
 
 

(Return)