DC-FSI using Radioss and AcuSolve

The following workflow is strongly recommended for solving DC-FSI problems:
  1. Develop Radioss structural model and an AcuSolve-only fluid model, and ensure that the uncoupled analyses run successfully.
  2. Prepare the stand-alone models that include DC-FSI commands.
  3. Run the coupled analysis.
  4. Post-process the FSI solution.

This workflow ensures that both the Radioss and the AcuSolve models are defined properly prior to performing a coupled simulation. Radioss and AcuSolve do not require that the analysis be run with a particular unit system, but both analyses need to use a consistent unit system. As a rule, all quantities exchanged between the two solvers will be in dimensional form, and the components of all vector quantities will be resolved in the inertial frame. For consistency, identical inertial frames must be selected for Radioss and AcuSolve.

Radioss Model

Preparing the Radioss model for DC-FSI involves three steps:
  1. Create input deck for Radioss
  2. Identify the interface region and the solution quantities exchanged
  3. Define the communication scheme
The Radioss FSI input data that has the Engine keyword /IMPL/DYNA/FSI is:

Each of the data items are discussed below under their relevant topic.

Damp Surfaces

The damp surface of the structural mesh must be specified in the Radioss FSI input data. The damp surface can either be specified by a group of elements or a surface. Note that the structural mesh on the damp surface does not have to match the interfacing fluid mesh. AcuSolve will internally project the CFD tractions from the fluid interface mesh onto a non-matching damp surface structural mesh. The mapping of nodal forces is also supported for structural beam elements. For example, a rod, pipe or blade can be modeled with simple beam elements in the structural mesh. The corresponding fluid mesh will contain the actual three-dimensional geometry of these beam elements.

If the damp surface is specified by a group of elements (ESET), use the /GRBEAM/BEAM/, /GRSHEL/SHEL/, or /GRSH3N/SH3N/ data for beam, 4-node, and 3-node shell elements, respectively. It is possible to specify the damp surface of a solid by coating it with shell elements and then assigning these elements zero material properties using the /MAT/LAW0 data. If the damp surface consists of beam elements, then these must be specified using the beam element group data. The ID of the element group is the first item of the /IMPL/DYNA/FSI data.

The damp surface (SSET) can also be specified by the Radioss /SURF data. The /SURF data has many options that can be used to specify a surface. The surface can be either the surface of a shell structure or the surface of a solid mesh. The surface ID is the second item of the /IMPL/DYNA/FSI data. Beam elements cannot be specified using the /SURF data.
Note: The damp surface can be defined by a combination of an element group and a surface.

The matching fluid surface is specified in the AcuSolve data using the EXTERNAL_CODE_SURFACE command.

In some cases a portion of the structural damp surface must be "tagged" so that AcuSolve can associate it with the AcuSolve boundary surface. This is done by specifying the Radioss part ID as the external_code_tags parameter in the EXTERNAL_CODE_SURFACE data.

         external_code_tags = {"10"}

Data is used to specify that this surface corresponds to the Radioss part with ID 10. Note that each individual surface must consist of elements with the same part ID, and each separate surface must consist of elements with separate part ID's. In order to apply a tag, the surface of a solid structure, the solid must be coated with shell elements and the property ID of these shell elements used as the surface tag. To specify the use of surface tags, set item 10 of the /IMPL/DYNA/FSI data (TAG) to 1.

AcuSolve Model

This section provides an overview for preparing the AcuSolve model for DC-FSI. For detailed information on the commands, refer to the AcuSolve Command Reference Manual. The three steps to prepare the AcuSolve model are:
  1. Set the analysis parameters to include an external field.
  2. Define the solution strategy.
  3. Define the external surface definition.

Analysis Parameter Setup to include an External Field

Use the EQUATION command to specify the solution fields available or the system of equation that are present in the problem. To include a field that is computed with an external solver, for Radioss, set the external_code parameter to 'ON'.

For example, when conducting a fluid-structure analysis in which AcuSolve computes the flow and Radioss computes displacements, turn ON the external_code parameter and allow for arbitrary mesh movement by setting the mesh parameter to arbitrary_lagrange_eulerian.
flow	= navier_stokes
mesh	= arbitrary_lagrange_eulerian
external_code	= on

Define Solution Strategy

In conjunction to the EQUATION command, which specifies the existence of solution fields in the problem, you must use TIME_SEQUENCE and STAGGER commands to define time stepping and staggering strategy. The preferred method is to use the AUTO_SOLUTION_STRATEGY command to have AcuSolve generate the solution strategy commands. In order to highlight the solution strategy commands, highlight the TIME_SEQUENCE and STAGGER commands.

The TIME_SEQUENCE command specifies the time stepping and staggering strategy. In the following example, the external field is solved first for structural displacements, which is then followed by the mesh displacement (ALE) in which the fluid elements are adjusted. Then the flow and turbulence equations are solved.
   min_time_steps                      = 1
   max_time_steps                      = 15
   min_stagger_iterations              = 1
   max_stagger_iterations              = 20
   staggers                            = { "external_code",
"turbulence" }
For each of the fields being solved (each stagger defined in the TIME_SEQUENCE command), you need to define the nonlinear iteration and linear solver parameters, using the STAGGER command. For example, the STAGGER commands are shown for external_code, mesh_displacement, and flow equations.
STAGGER ( "external_code” ) {
   equation                            = external_code
   min_stagger_iterations              = 1
   max_stagger_iterations              = 10
STAGGER( "mesh_displacement" ) {
   equation                            = mesh_displacement
   min_stagger_iterations              = 1
   max_stagger_iterations              = 5
   convergence_tolerance               = 0.1
   linear_solver                       = conjugate_gradient
   min_linear_solver_iterations        = 10
   max_linear_solver_iterations        = 1000
   linear_solver_tolerance             = 0.001
   projection                          = off
STAGGER( "flow" ) {
   equation                            = flow
   min_stagger_iterations              = 1
   max_stagger_iterations              = 2
   convergence_tolerance               = 0.1
   lhs_update_frequency                = 1
   linear_solver                       = gmres
   linear_solver_tolerance             = 0.1

Define Fluid-Structure Interface

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

In the following example, the interface surface topology is read from the file wall.ebc located in the MESH.DIR directory and consists of 3-node triangles. The velocity_type, temperature_type, and mesh_displacement_type define the interface properties (boundary conditions) and are:
   surfaces	= Read( "MESH.DIR/wall.ebc" )
   shape            	= "three_node_triangle"
   element_set	= "tet fluid"
   velocity_type	= wall
   temperature_type	= tied
   mesh_displacement_type  	= tied
   gap	= 0
   gap_factor	= 0
   external_code_tags	= {}

The interface properties or boundary conditions are specified through the mesh_displacement_type, velocity_type, and temperature_type parameters. 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.

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. Direct-Coupled Fluid-Structure Interaction Boundary Conditions
Fluid-Solid Interface Conditions Mesh Displacement
Tied Slip
Velocity Type Wall x f l u i d = x s o l i d

u f l u i d = ( x f l u i d n + 1 x f l u i d n ) / Δ t

x f l u i d S s o l i d

u f l u i d n = ( x f l u i d n + 1 x f l u i d n ) / Δ t n

u f l u i d t i = ( x s o l i d n + 1 x s o l i d n ) / Δ t t i i = 1 , 2

Slip x f l u i d = x s o l i d

u f l u i d n = ( x f l u i d n + 1 x f l u i d n ) / Δ t n

x f l u i d S s o l i d

u f l u i d n = ( x f l u i d n + 1 x f l u i d n ) / Δ t n

When the fluid is allowed to slide along the solid mesh, neighborhood searches between the fluid and solid meshes are continuous 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 specified a dimensional maximum gap distance between each quadrature point of the AcuSolve surface to the closest surface given by Radioss to check for gaps. If the distance is greater than the gap, the computation stops with an error message.