# Structural Fluid-Structure Interaction Analysis

OptiStruct and AcuSolve are fully-integrated to perform a coupled Fluid-Structure Interaction Analysis based on a partitioned staggered approach.

OptiStruct and AcuSolve both include time-domain simulation capabilities that break the coupled solution into a number of time steps. Since the governing equations of both OptiStruct and AcuSolve are nonlinear, sub-iterations are typically required within each time step. For more information, refer to the Fluid-Structure Interaction in the User Guide. This document illustrates the Structural Fluid-Structure Interaction based on Nonlinear Direct Transient Analysis in the structural domain (OptiStruct) and transient fluid flow analysis in the fluid domain (AcuSolve). SFSI is used to denote Structural Fluid-Structure Interaction and TFSI is used to denote Thermal Fluid-Structure Interaction.
At each sub-iteration (exchanges/staggers) of SFSI analysis, the nodal general force at the fluid-structure interface is passed from AcuSolve to OptiStruct, becoming part of the loading for the solution in OptiStruct. On the other hand, displacement from OptiStruct at the interface is converted into velocity and imposed as boundary conditions for the flow solution in AcuSolve.
Note: In addition to the load imposed by the flow, additional structural loads can also be applied. This SFSI cycle is shown in Figure 1.

## Input/Output

The detailed interface-specific input information is available in the Fluid-Structure Interaction page. Here you will look at solution-specific information required to run Structural FSI.

First look at the input data required from the OptiStruct side to set up the model. Subsequently, some information about the interface boundary conditions that are specific to Structural FSI is explained and to learn how to set them in the AcuSolve input file.

### OptiStruct

Structural FSI is the coupled simulation of Nonlinear Direct Transient Analysis on the structure in conjunction with dynamic fluid flow analysis in the fluid domain.

Refer to Nonlinear Direct Transient Analysis in the User Guide for detailed information regarding the setup of the OptiStruct model. There are a few changes you will need to make to the model to run FSI. Look at these differences in the following points:
1. The initial time step (DT on NLPARM or TSTEPNL) should be set equal to the initial time step in the AcuSolve model. Fixed time step will be enforced throughout the solution and this will also be equal to the initial time step (adaptive time stepping is not supported).
2. The FSI Bulk Data Entry should be added to the model. You can adjust the convergence tolerance parameters relevant to Structural FSI (FCNVTOL and DCNVTOL), the wait time (WAITTIME), and other parameters on this entry.
3. The FSI Subcase Information Entry should be added to the nonlinear direct transient subcase and this entry should reference the corresponding FSI Bulk Data Entry.

The above steps allow you to successfully prepare the Nonlinear Transient Model for FSI analysis.

### AcuSolve

Structural FSI is a coupling between the structural solver and the dynamic fluid flow analysis capabilities of the fluid solver. Therefore, you can look at the AcuSolve Command Reference Manual for detailed information about how to set up a model for dynamic fluid flow solutions. The deformations of the structural interface may lead to changes in fluid flow that affects the subsequent solution. Here a few parameters relevant to Structural FSI in the AcuSolve input file are looked at.

Use the EXTERNAL_CODE_SURFACE command to define the interaction between the fluid interface and the corresponding parameters. The command specifies the surface topology, as well as the interface proprieties.

Depending on the problem being solved (SFSI or TFSI), various parameters are available to define the interface behavior. For detailed information on the different parameters, refer to the AcuSolve Command Reference Manual.
EXTERNAL_CODE_SURFACE( "<structure_label>" ) {
shape                               = "<element type>"
element_set                         = "<element set ID>"
velocity_type                       = <wall/slip>
mesh_displacement_type              = <tied/slip>
gap_factor                          = <Real>
gap                                 = <Real>
}

For Structural FSI, the velocity_type and mesh_displacement_type define how the fluid and structural interfaces interact (boundary conditions). The mesh_displacement parameter defines whether the fluid mesh is tied to the solid mesh or allowed to slip against the solid mesh surface. Set the mesh_displacement_type=tied to tie the fluid mesh to the solid mesh, or mesh_displacement_type=slip to allow the fluid mesh to slide against the solid surface, which acts as a guide surface. For Structural FSI, there is exchange of displacements and pressure at the interface and in addition, mesh displacement and velocity boundary conditions are present. Therefore, the mesh parameter should be set to Arbitrary Lagrangian Eulerian. For more information, refer to External Equation Field Settings of the Fluid Structure Interaction page.

The velocity_type specifies how the fluid velocity behaves in relation to the structural mesh velocity. Set velocity_type=wall to tie the fluid velocity to the mesh velocity, or set velocity_type=slip for the normal component of the fluid velocity to be tied to the solid mesh velocity.

There are four possible interface combinations based on the settings of the mesh_displacement and velocity_type parameters. These are summarized in Table 1.
Table 1. Fluid-Structure Interaction Boundary Conditions
Fluid-Solid Interface Conditions Mesh Displacement
Tied Slip
Velocity Wall Mesh Displacement:

${u}_{fluid}={u}_{solid}$

Mesh Displacement:

${u}_{fluid}\ne {u}_{solid}$

Velocity:

${v}_{fluid}=\frac{{u}_{fluid}^{n+1}-{u}_{fluid}^{n}}{{t}^{n+1}-{t}^{n}}$

Velocity:

${v}_{fluid}·\stackrel{^}{n}=\left(\frac{{u}_{solid}^{n+1}-{u}_{solid}^{n}}{{t}^{n+1}-{t}^{n}}\right)·\stackrel{^}{n}$

${v}_{fluid}·\stackrel{^}{t}=\left(\frac{{u}_{solid}^{n+1}-{u}_{solid}^{n}}{{t}^{n+1}-{t}^{n}}\right)·\stackrel{^}{t}$

Slip Mesh Displacement:

${u}_{fluid}={u}_{solid}$

Mesh Displacement:

${u}_{fluid}\ne {u}_{solid}$

Velocity:

${v}_{fluid}·\stackrel{^}{n}=\left(\frac{{u}_{fluid}^{n+1}-{u}_{fluid}^{n}}{{t}^{n+1}-{t}^{n}}\right)·\stackrel{^}{n}$

Velocity:

${v}_{fluid}·\stackrel{^}{n}=\left(\frac{{u}_{solid}^{n+1}-{u}_{solid}^{n}}{{t}^{n+1}-{t}^{n}}\right)·\stackrel{^}{n}$

Where,
$\stackrel{^}{n}$
Normal unit vector at the interface.
$\stackrel{^}{t}$
Translational unit vector at the interface.
There are two translational unit vectors in the 2-dimensional plane of the interface.
Note: For the velocity=slip condition, the velocity in translational direction is not constrained at the interface.

When the fluid is allowed to slide along the solid mesh, neighborhood searches between the fluid and solid meshes are continuously performed. The gap_factor parameter specifies a non-dimensional (with respect to the length of the element face) maximum allowable gap and the gap parameter specifies a non-dimensional maximum gap distance between each quadrature point of the AcuSolve surface to the closest surface given by OptiStruct to check for gaps. If the distance is greater than the gap, the computation stops with an error message.

### Output

The FSI results are output to the corresponding working directories. The structural (OptiStruct) results are output to the H3D file by default and can be post-processed in HyperView. However, this file will not contain the fluid results. The fluid results are available in the AcuSolve .log file in the AcuSolve working directory. The AcuSolve .log file can also be loaded into HyperView.

For Structural FSI, currently, the fluid and structural results may be imported into a single HyperView session by choosing the overlay option. Only results common to both the structural and fluid analyses are available to be post-processed simultaneously.

The structural solution can be viewed in HyperView by opening the H3D file as illustrated in Figure 2.

You can overlay (check the Overlay box in the HyperView Load Model and Results panel) the fluid results by loading the AcuSolve .log file in Figure 2. However, since there are no common result labels, currently, you can only post-process one set of results in any single session.