CFD-ACE Interface

S

(Return)

The translator creates the CFD-ACE grid and physical data files. It supports 2D or 3D configurations composed of single or multiblock grid. Non C0-contiguous interfaces are supported for both 2D and 3D configurations. The grid file is written in PLOT3D multigrid format with iblank array. It can be written in single (default) or double precision. The supported iblank values are:

• 1 : normal fluid nodes
• 2 : solid wall boundary
• -n = space continues on block n.

The physical data file contains three sections:

• Boundary condition locations and physical data values
• Cell type information
• Domain connectivity information

Creating the CFD-ACE input files

The translator writes the CFD-ACE mesh file using the selected structured domain files, the boundary conditions file and the topology file. To create the CFD-ACE mesh file, select the translator "CFD-ACE" in the "Output" menu from the ICEM CFD/CAE Manager. After clicking "Write output" you can specify the following options for the CFD-ACE interface:

• select the domains to include in the output mesh
• give the name of the boundary condition file (default is configuration/parts_mesh/mesh/boco)
• give the name of the topology file (default is configuration/topology/topo_mulcad_out)
• option to write only the grid file
• option to write only the physical data file
• option to create the grid file in double precision
• give the name of the CFD-ACE file(s)
  (default: configuration/parts_mesh/transfer/configuration.grid
  (default: configuration/parts_mesh/transfer/configuration.phys
  

The interface generates the CFD-ACE mesh file located in the Transfer Shell. You may open a shell window in this directory by selecting the menu items "Utility" and "Transfer Shell".

Defining boundary conditions in MULCAD

This interface has a special menu in MULCAD for defining boundary conditions. To display the CFD-ACE special menu, set the analysis code to CFD-ACE in MULCAD:

Select the menu ANALYSIS from the ICEM CFD/CAE MULCAD main menu.

• Define the analysis code:
  • select 1. MODALS
  • select 1. ANALYSIS CODE CFD-ACE
• Set the boundary condition data:
  • select SET BOUND. COND. DATA
    • select SUBFACES for 3D models
    • select EDGE ENTITIES for 2D models
  • select subfaces or edge entities.

The available boundary conditions are:

1. UNSPEC. BOUND. COND.
2. BC_TYPE: INLET
3. BC_TYPE: EXIT_P
4. BC_TYPE: SYMMETRY
5. BC_TYPE: WALL
6. BC_TYPE: EXIT_E
7. BC_TYPE: EXIT_C
8. VELOCITY: velocity component in x, y and z directions
9. TURBULENT QUANTITIES
   • First turbulent kinetic energy (TK1)
   • Dissipation of first turbulent energy (TD1)
   • Length scale for turbulence
10. TOTAL ENTHALPY: value of total enthalpy
11. COMPOSITION: Scalar composition number
12. PRESSURE: Value of pressure
13. TEMPERATURE: Value of temperature

In this menu, specify the boundary condition types (options 2 to 7) and boundary condition values (options 8 to 13). The first option (1.UNSPEC. BOUND.COND) allows the user to define his own boundary condition type flags.

Defining cell types and properties in MULCAD

With the ANALYSIS CODE set to CFD-ACE, the following menu appears when a domain is selected:

1. UNSPEC BOUND. COND.
2. CELL_TYPE: BLOCKED
3. CELL_TYPE: HEAT TRANSFER
4. THERMAL CONDUCTIVITY
5. SPECIFIC HEAT
6. DENSITY
7. INITIAL TEMPERATURE
8. MELTING TEMPERATURE
9. LATENT HEAT

This menu allows to specify the cell type (options 2 and 3) and the cell properties (options 4 to 9). The translator supports the cell type information only for whole domains, not for subdomains.

Defining boundary conditions in the DDN-Mesher Interface

For grids generated with the HEXA-Mesher, the boundary conditions and properties are defined in the "general bound. cond." menu of the DDN-Mesher Interface. Please refer to the General Remarks section for more details.

Boundary condition type:

In the DDN-Mesher Interface, select a boundary family (surface in 3D or edge in 2D) and give it one of the following flags (string1) in the property menu:

    string1		Description
    -------		-----------
    INLET		BC-Type Inlet
    OUTLT		BC-Type Exit_P
    SYMM		BC-Type Symmetry
    WALL		BC-Type Wall
    EXTR		BC-Type Exit_E
    FIXX		BC-Type Exit_C

Boundary condition values:

    VELOCITY:
    1.string1		VELO
    3.integer		Enter the X-component of the velocity
    4.real1		Enter the Y-component of the velocity
    5.real2		Enter the Z-component of the velocity

    TURBULENT QUANTITIES:
    1.string1           TUEN
    3.integer           Enter the first turbulent kinetic energy
    4.real1             Enter the dissipation of the first turbulent energy
    5.real2             Enter the length scale for turbulence

    TOTAL ENTHALPY:
    1.string1           ENTH
    3.integer           Enter the total enthalpy

    COMPOSITION:
    1.string1           FRAC
    3.integer           Enter the scalar composition number

    PRESSURE:
    1.string1           PRES
    3.integer           Enter the pressure

    TEMPERATURE:
    1.string1           TEMP
    3.integer           Enter the temperature

Defining cell types and properties in the DDN-Mesher Interface

Cell type:

The cell type can only be assigned to blocks in 3D or faces in 2D. Two cell types are available:

    1.string1           BLOCK	For cell type:  Blocked
    1.string1           HEATT	For cell type:  Heat transfer

Cell properties:

    THERMAL CONDUCTIVITY:
    1.string1           THCON
    3.integer           Enter the thermal conductivity

    SPECIFIC HEAT:
    1.string1           CP
    3.integer           Enter the specific heat

    DENSITY:
    1.string1           DENS
    3.integer           Enter the density

    INITIAL TEMPERATURE:
    1.string1           TEMPI
    3.integer           Enter the initial temperature

    MELTING TEMPERATURE:
    1.string1           TEMPM
    3.integer           Enter the melting temperature

    LATENT HEAT:
    1.string1           HL
    3.integer           Enter the latent heat

Note that a real value can be defined in the field "integer" of the DDN-Mesher Interface.

(Return)