### 1.2.10. Immersed Solids

The Immersed Solids capability of ANSYS CFX enables you to model steady-state or transient simulations involving rigid solid objects that can move through fluid domains. The model involves the use of an immersed solid domain that is placed inside a fluid domain. As a simulation proceeds, CFX-Solver applies a source of momentum to the fluid inside the immersed solid domain in order to force the flow to move with the solid.

In a parallel run, all partitions hold a copy of the entire mesh of the immersed solid domain. This facilitates the parallelization of the intersection process and eliminates unnecessary communications.

Steps to create an immersed solid:

1. Define an immersed solid domain to represent the solid. For details, see Domain Type in the CFX-Pre User's Guide.

   This domain should be entirely or partly within a fluid domain. Care must be taken to ensure that the immersed solid domain does not cross any fluid boundaries or collide with any solid domains or immersed solid domains. An immersed solid domain should not cross any GGI interface that involves a non-stationary domain. Do not create a domain interface between the immersed solid domain and the fluid domain.

2. Specify the Domain Motion settings for the immersed solid domain in order to prescribe the motion of the immersed solid. For details, see Domain Motion in the CFX-Pre User's Guide.

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.

For problems that have convergence difficulties, you can try using better initial conditions. You can obtain initial conditions by using one of the following methods:

- Run a case with Momentum Source Scaling Factor set to zero or a very small value (for example, less than 1.0).

- Run a stationary case and use the results to initialize a moving immersed solid case.

Once you have good initial conditions, you can improve the stability of the solution by using one of the following methods:

- Use the `inside()` function to initialize the flow field so that the flow inside the immersed solid moves with the immersed solid.

- Use a tighter convergence criterion and enable more coefficient loops per time step.

When you postprocess a simulation that involves an immersed solid, the results file and any full transient results files contain a variable named “Inside [domain name]”. This variable is set to 1 for mesh nodes inside the immersed solid, and 0 for mesh nodes outside the immersed solid.

Variables used for plots or calculations on immersed solid domain boundaries are not taken from the immersed solid domain; instead, they are interpolated from the fluid/porous domain in which the solid is immersed. The accuracy of such interpolation is dependent on the mesh densities of both the fluid/porous domain and the surface of the immersed solid domain. To visualize, or perform computations with, variables that are associated with the immersed solid domain, use slice planes, user surfaces, or other locators that are offset into the immersed solid domain, and set the applicable Domains setting to refer to the immersed solid domain.

Note: CFD-Post does not add viscous stresses to the evaluation of variables or expressions on immersed solid surfaces. Thus, using CFX-Solver Manager to monitor "force()@Immersed solid" (where ’Immersed solid’ is the name you have given to a surface) gives a different result to calculating "force()@Immersed solid" in CFD-Post.

#### 1.2.10.1. Immersed Boundary Tracking

By default, the fluid just outside an immersed boundary has no forcing terms to account for the boundary layer or other effects of the boundary on the flow. To better resolve these boundary effects, CFX-Solver can impose a modified forcing term near the immersed boundary. To activate these forcing terms, visit the Immersed Solid Control settings (see Immersed Solid Control in the CFX-Pre User's Guide), then set Boundary Model to `Modified Forcing` and set the Boundary Tracking settings.

In order for CFX-Solver to calculate the forcing terms, the nearest point on the immersed boundary must be identified for each near-wall node (see Notation in the CFX-Solver Theory Guide). This involves using one of two search algorithms. Which search algorithm is used depends on which option is selected for the Boundary Tracking setting: `Search Through Elements` or `Boundary Face Extrusion`.

The search algorithm that is used when the Boundary Tracking setting is `Boundary Face Extrusion` has the advantage of finding the wall normal direction in physical space (as opposed to computational space), but the success of this algorithm depends on the distance that the boundary face is extruded along the wall normal direction.

When using the `Search Through Elements` method, it is important to have the immersed solid mesh element lengths larger in the direction normal to the immersed boundary than the fluid mesh element lengths near the immersed boundary, so that the in-wall nodes tend to fall within the outer layer of immersed solid boundary 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. The weakness of this option is that the projection is done in the computational space so that, compared to the other option, the normal direction is generally less accurate.

When using the `Boundary Face Extrusion` method, it is important to have the extrusion distance larger than the fluid mesh element lengths near the immersed boundary, to ensure that the near-wall nodes fall within the bounding boxes of the imaginary volumes extruded from the immersed boundary face. When using this option, CFX-Solver will search through fluid nodes near the immersed boundary and project the near-immersed-boundary fluid nodes onto the faces or edges of the immersed boundary, with the projection being carried out in physical space. Because the projections are done in physical space, as opposed to computational space, accuracy is better than that of the `Search Through Elements` option.

#### 1.2.10.2. Limitations to using Immersed Solids

The following modeling restrictions and limitations apply to simulations involving immersed solids:

- An immersed solid domain cannot undergo mesh deformation.

- An immersed solid domain cannot model heat transfer.

- When modeling an immersed solid governed by the rigid body solver, you cannot set initial conditions.

- A fluid domain that contains (or partly contains) an immersed solid domain cannot support many modeling options, including:

  - heat transfer

  - Additional Variables

  - combustion

- For transient cases, immersed solids do not interact properly with fluid domains that involve compressibility or multiphase flow.

- For steady-state simulations, if the immersed solid is moving, the motion must not have any normal component.

- The solid surfaces of an immersed solid are not explicitly resolved by the mesh. In addition, a wall function cannot be applied to the boundary of an immersed solid. As a consequence, the quality of simulation results may be lower than can be obtained using mesh deformation or other techniques that support the use of wall boundaries to directly resolve solid surfaces.

  In general, the mesh for the immersed solid should be sufficiently fine on the boundaries to resolve the shape of the boundary surface; the mesh inside the immersed solid may be arbitrarily coarse. The fluid mesh around the immersed solid should be fine enough to enable effective interpolation of near-immersed-boundary fluid nodes onto the immersed solid. It is advised that you have at least 10 fluid domain elements on either side of the immersed solid boundary.

- Particles do not interact with the walls of an immersed solid domain; particles are tracked inside an immersed solid domain based on the fluid velocity, which is driven to match the velocity of the immersed solid domain.

- When an immersed solid straddles or crosses a periodic interface, it is not automatically replicated by the solver. If you expect this to happen, make additional copies of the immersed solid as necessary.

- If an immersed solid case is run in parallel, in some cases (including some rigid body cases) the path taken to convergence is sensitive to the number or placement of partitions, although the converged results are unaffected. You should ensure that a steady-state simulation, or each time step in a transient simulation, is sufficiently well-converged to avoid differences in results between runs with different parallel run settings.

- If an immersed solid boundary coincides with a GGI interface during a parallel run, the results of the immersed solid case may vary slightly depending on the number of partitions. This is because the solver does not assemble a coefficient matrix on the overlapping elements, and the Rhie Chow coefficients will therefore not take into account the contributions of the immersed solids on the overlapping elements.

- The immersed solid `Modified Forcing` method is targeted at predicting turbulence for the standard k-epsilon () and the Shear Stress Transport (SST) models only. While other two-equation turbulence models can be used with immersed solids, turbulence predictions may not be accurate. The Modified Forcing method cannot be used with turbulence models that are not two-equation models (for example, Reynolds stress models, LES models, EARSM models, Zero Equation and Eddy Viscosity Transport Equation, and so on). Regardless of the immersed solid settings used, you should ensure that you understand the limitations of the accuracy of the immersed solids model in predicting turbulence for your particular application. This limitation also applies to using the `Modified Forcing` option with scalable wall functions for low Reynolds number cases.

- Except for force and torque callbacks, CEL callbacks are not supported on immersed boundaries.

- CEL callbacks for force and torque on an immersed boundary or region are not supported for rotating fluid domains.

- The force and torque callback functions may not be accurate. When calculating forces and torques on an immersed solid, the viscous contribution is typically underestimated. This is also the case when forces and torques are calculated on a rigid-body immersed solid. The accuracy of the force and torque information passed to the rigid body solver depends on the details on the problem set up, and is affected by the near-wall flow predictions. Also, callback results for forces and torques may differ on an immersed solid region from those on an immersed boundary because wall shear is not included when using a mesh region. The forces and torques calculated on immersed solids will differ between CFD-Post and CFX-Solver.

- If a fluid region or boundary intersects with an immersed solid, any callback function on that fluid region or boundary will not take into account the presence of the immersed solid.

- For low Reynolds number turbulence cases, the immersed solids turbulence model cannot accurately predict the pressure fields near the immersed boundaries.

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