ICFD Setup Script
ICFD Setup Script
The Incompressible Computational Fluid Dynamics (ICFD) solver can be used to simulate fluid flow problems where the fluid can be assumed to be incompressible. The solver can be used on its own, or it can be coupled to the solid mechanics or thermal solvers.
This ICFD model setup script enables the user to create a simple ICFD model from selected shell parts which represent the fluid boundaries. The user also has the option to generate far field boundaries around a part by selecting a central part and specifying the distances to the boundaries from this central part.
The model generated by this panel is a simple one and only a limited number of the ICFD features are used. However, a user wishing to create a more complex model may want to use this script to create a simple model first before adding complexity through the PRIMER keyword menu.
The following figure shows the input panel of the ICFD model setup script:
The first section of the input panel (highlighted in box 1 above) creates shell parts which are to be used as far field boundaries. Six shell parts are created, one for each direction, and the parts are made up of shell elements. The creation of far field boundaries may be required if a user has a part over which they wish to simulate the external flow (e.g. the airfoil shown in the figure). If the user already has all the shell parts defining the fluid boundary, then this section can be skipped.
The far field boundary generation can be activated by clicking the tick button at the top of section 1 in the figure above. The following options are available in the first section:
| Central Part | This is a part which is used as a reference for creating the far field boundaries. |
| Distances to far field boundaries | These are the distances between the central reference part and the far field boundaries. Six values are required in this table, with one distance for each direction (negative x, positive x, negative y, positive y, negative z, positive z). The distances are measured from the closest node on the central reference part e.g. the minimum x coordinate of the part is used for the distance to the negative x boundary far field. |
| Mesh size | This is the mesh size on the far field boundaries. Select a large mesh size initially before reducing it if required. |
The second section of the input panel (highlighted in box 2 above) enables the user to create an ICFD model from shell parts. These parts can be those created in section 1 of the input panel, or pre-existing shell parts. The ICFD model will be generated as a separate new model.
The input table is used to input the numbers of shell parts and the ICFD boundary information. The following information must be specified on each row:
| Type |
Select one of the following:
Inlet
Outlet
No-slip wall
Slip wall
|
| Part | The ID of the shell part to be used as the boundary. An *ICFD_PART is created for each part, each shell element is translated into a *MESH_SURFACE_ELEMENT and each node is translated into a *MESH_NODE. |
| Vx, Vy, Vz | For Inlet type boundaries, these are the velocity components in the x, y and z directions. |
| p | For Outlet type boundaries, this is the prescribed relative pressure (zero for atmospheric conditions). |
| nlayer | For No-slip wall and Slip wall type boundaries, this is the number of mesh boundary layer cells. *MESH_BL_SYM cards are automatically added to inlet and outlet boundaries. This ensures that the boundary layer cells continue all the way to the inlet or outlet boundaries. |
| forces | For No-slip wall and Slip wall type boundaries, this box can be ticked to output the fluid force time history *ICFD_DATABASE_DRAG. |
The number of rows in the table can be changed by either clicking the "Delete" button at the right-hand side of each row or by editing the "Number of boundaries" field just above the table.
To create an ICFD model, the ICFD fluid volume must be entirely enclosed by the boundaries, with no holes and no duplicate nodes at the edges. The "Check for holes" button can be used to check if this is the case.
Once the boundaries have been written to this table, and checked for holes, some essential parameters must be entered before the ICFD model can be generated (section 3 in the figure above):
| Density | This is the fluid density to be used in the *ICFD_MAT card. |
| Kinematic viscosity | This is the fluid kinematic viscosity to be used in the *ICFD_MAT card. |
| Fluid simulation | This is the ICFD simulation end time to be used in the *ICFD_CONTROL_TIME card. |
| D3PLOT output period | This is the time interval between states to be used in the *DATABASE_BINARY_D3PLOT card. |
Once values have been inputted for these parameters, click "Generate ICFD model". This will create a new model with all the cards required to run a simple ICFD simulation. ICFD models must be run in a double precision solver.