### 20.1.4. Immersed Solid Control

The immersed solid is represented as a source term in the fluid equations that drives the fluid velocity to match the solid velocity. The size of the source term is controlled by the Momentum Source Scaling Factor setting, which can be set globally (in the global Solver Control settings) or for individual immersed solids (on the immersed solid domain Solver Control tab). The default value of 10 is acceptable most of the time. If robustness problems are encountered, the scaling factor may be decreased (for example by a factor of 2), but at the expense of accuracy; the difference between the fluid velocity and the specified solid velocity will generally increase, even if only by a small amount.

Boundary Model has two options:

- `None`

  This is the default option.

- `Modified Forcing`

  This option enables modifications to the immersed solid source term to take better account of the boundaries of the immersed solid and their effect on the flow.

If you set Boundary Model to `Modified Forcing`, then the Boundary Tracking setting is available.

The Boundary Tracking setting has two options:

- `Boundary Face Extrusion`

  Once Boundary Model is selected, this is the default option.

  The `Boundary Face Extrusion` option requires you to specify two settings that must be set appropriately so that each near-wall node can be reliably projected onto the best location on the immersed boundary face. These settings are:

  - Extrusion Distance

    This is the distance by which each immersed boundary face is extruded outward from, and normal to, the immersed boundary to form an imaginary volume. A bounding box, that consists of faces of constant x, y, and z coordinate, is then constructed around each imaginary volume. If a near-wall node falls within the bounding box, then CFX-Solver will project that near-wall node normal to and onto the plane of the boundary face. If the projected location lies outside the face, other mechanisms take effect to find the nearest suitable projected location.

    The value of Extrusion Distance should be of the order of magnitude of the length of a fluid mesh element in the vicinity of the immersed boundary.

  - Extrusion Tolerance

    This is a factor by which the solver will multiply the edge length of the bounding box for each imaginary volume. The bounding box is mentioned in the description for the Extrusion Distance setting. An overly large value will cause near-wall nodes to be mapped to locations on boundary faces that are not necessarily the closest face.

    The default value for Extrusion Tolerance is `0.01`.

- `Search Through Elements`

  When using this option, CFX-Solver will search through elements near the immersed boundary and project the near-immersed-boundary fluid nodes onto the face edge or vertices of the immersed solid element. This option requires no user input.

  This method is less accurate than the `Boundary Face Extrusion` option, but can be used for cases where no suitable Extrusion Distance can be determined.

For details, see Immersed Boundary Tracking in the CFX-Solver Modeling Guide.

Release 18.2 - © ANSYS, Inc. All rights reserved.